(2014) Finite Element Analysis and Design of Metal Structures - Ehab Ellobody, Ran Feng and Ben Young

Prévia do material em texto

Finite Element Analysis and
DESIGN OF METAL
STRUCTURES
This page intentionally left blank
Finite Element Analysis and
DESIGN OF METAL
STRUCTURES
EHAB ELLOBODY
RAN FENG
BEN YOUNG
AMSTERDAM • BOSTON • HEIDELBERG • LONDON
NEW YORK • OXFORD • PARIS • SAN DIEGO
SAN FRANCISCO • SINGAPORE • SYDNEY • TOKYO
Butterworth-Heinemann is an imprint of Elsevier
Butterworth-Heinemann is an imprint of Elsevier
225 Wyman Street, Waltham, MA 02451, USA
The Boulevard, Langford Lane, Kidlington, Oxford OX5 1GB, UK
Copyright r 2014 Elsevier Inc. All rights reserved.
No part of this publication may be reproduced, stored in a retrieval
system, or transmitted in any form or by any means, electronic, mechanical,
photocopying, recording, or otherwise, without the prior written
permission of the publisher.
Permissions may be sought directly from Elsevier’s Science & Technology
Rights Department in Oxford, UK: (144) 1865 843830, fax: (144) 1865
853333, e-mail: permissions@elsevier.co.uk. You may also complete your
request on-by visiting the Elsevier web site at http://elsevier.com/locate/
permissions, and selecting Obtaining permission to use Elsevier material
Library of Congress Cataloging-in-Publication Data
A catalog record for this book is available from the Library of Congress.
British Library Cataloguing-in-Publication Data
A catalogue record for this book is available from the British Library.
ISBN: 978-0-12-416561-8
For information on all Butterworth-Heinemann publications
Visit our Web site at www.books.elsevier.com
13 14 15 16 17 10 9 8 7 6 5 4 3 2 1
Printed in the United States of America
mailto:permissions@elsevier.co.uk
http://elsevier.com/locate/permissions
http://elsevier.com/locate/permissions
http://www.books.elsevier.com
CONTENTS
1. Introduction 1
1.1. General Remarks 1
1.2. Types of Metal Structures 3
1.3. Experimental Investigations and Its Role for Finite Element Modeling 7
1.4. Finite Element Modeling of Metal Structures 9
1.5. Current Design Codes 11
References 13
2. Review of the General Steps of Finite Element Analysis 15
2.1. General Remarks 15
2.2. Dividing and Selection of Element Types for Metal Structures 17
2.3. Selection of a Displacement Function 23
2.4. Definition of the Strain�Displacement and Stress�Strain Relationships 23
2.5. Derivation of the Element Stiffness Matrix and Equations 24
2.6. Assemblage of Element Equations 24
2.7. Solving the Assembled Equations for the Unknowns 25
References 30
3. Finite Element Modeling 31
3.1. General Remarks 31
3.2. Choice of Element Type for Metal Structures 32
3.3. Choice of Finite Element Mesh for Metal Structures 40
3.4. Material Modeling 43
3.5. Modeling of Initial Imperfections 46
3.6. Modeling of Residual Stresses 48
3.7. Load Application 52
3.8. Boundary Conditions 53
References 54
4. Linear and Nonlinear Finite Element Analyses 56
4.1. General Remarks 56
4.2. Analysis Procedures 58
4.3. Linear Eigenvalue Buckling Analysis 62
4.4. Materially Nonlinear Analysis 65
4.5. Geometrically Nonlinear Analysis 67
v
4.6. Riks Method 68
References 71
5. Examples of Finite Element Models of Metal Columns 72
5.1. General Remarks 72
5.2. Previous Work 73
5.3. Finite Element Modeling and Example 1 80
5.4. Finite Element Modeling and Example 2 86
5.5. Finite Element Modeling and Example 3 90
5.6. Finite Element Modeling and Example 4 100
References 112
6. Examples of Finite Element Models of Metal Beams 115
6.1. General Remarks 115
6.2. Previous Work 116
6.3. Finite Element Modeling and Results of Example 1 126
6.4. Finite Element Modeling and Results of Example 2 130
6.5. Finite Element Modeling and Results of Example 3 135
References 148
7. Examples of Finite Element Models of Metal Tubular Connections 151
7.1. General Remarks 151
7.2. Previous Work 154
7.3. Experimental Investigations of Metal Tubular Connections 160
7.4. Finite Element Modeling of Metal Tubular Connections 171
7.5. Verification of Finite Element Models 175
7.6. Summary 179
References 180
8. Design Examples of Metal Tubular Connections 182
8.1. General Remarks 182
8.2. Parametric Study of Metal Tubular Connections 183
8.3. Design Rules of Metal Tubular Connections 185
8.4. Comparison of Experimental and Numerical Results with
Design Calculations 189
8.5. Design Examples 190
8.6. Summary 204
References 205
Index 207
vi Contents
CHAPTER11
Introduction
1.1. GENERAL REMARKS
Most of finite element books available in the literature, e.g. Refs [1.1�1.7],
deal with explanation of finite element method as a widely used numerical
technique for solving problems in engineering and mathematical physics.
The books mentioned in Refs [1.1�1.7] were written to provide basic learn-
ing tools for students in civil and mechanical engineering. The aforemen-
tioned books highlighted the general principles of finite element method and
the application of method to solve practical problems. Numerous books are
also available in the literature, as examples in Refs [1.8�1.26], addressing the
behavior and design of metal structures. The books mentioned in Refs
[1.8�1.26] have detailed the analysis and design of metal structural elements
considering different design approaches. However, up-to-date, there is a
dearth in the books that detail and highlight the implementation of finite ele-
ment method in analyzing metal structures. Extensive numerical investiga-
tions using finite element method were presented in the literature as research
papers on metal columns, beams, beam columns, and connections. However,
detailed books that discuss the general steps of finite element method specifi-
cally as a complete work on metal structures and connections are rarely found
in the literature, leading to the work presented in this book.
There are many problems and issues associated with modeling of metal
structures in the literature that students, researchers, designers, and aca-
demics need to address. This book provides a collective material for the
use of finite element method in understanding the behavior and structural
performance of metal structures. Current design rules and specifications
of metal structures are mainly based on experimental investigations,
which are costly and time consuming. Hence, extensive numerical inves-
tigations were performed in the literature to generate more data, fill in
the gaps, and compensate the lack of data. This book also highlights the
use of finite element methods to improve and propose more accurate
design guides for metal structures, which is rarely found in the literature.
The book contains examples for finite element models developed for
1
Finite Element Analysis and Design of Metal Structures
DOI: http://dx.doi.org/10.1016/B978-0-12-416561-8.00001-9
© 2014 Elsevier Inc.
All rights reserved.
http://dx.doi.org/10.1016/B978-0-12-416561-8.00001-9
different metal structures as well as worked design examples for metal
structures. The authors hope that this book will provide the necessary
material for all interested researchers in the field of metal structures. The
book can also act as a useful teaching tool and help beginners in the field
of finite element analysis of metal structures. The book can provide a
robust approach for finite element analysis of metal structures that can be
understood by undergraduate and postgraduate students.
The book consists of eight well-designed chapters covering necessary
topics related to finite element analysis and design of metal structures.
Chapter 1 provides a general background for the types of metal structures,
mainly on columns, beams, and tubular connections. The three topics pres-
ent the main structural components that form any metal frame, building,
or construction. Detailing the analysis of these components would enable
understanding the overall structural behavior of different metal structures.
The chapter also gives a brief review of the role of experimental investiga-
tions as thebasis for finite element analysis. Finally, the chapter highlights
the importance of finite element modeling and current design codes for
understanding the structural performance of metal structures.
Chapter 2 provides a simplified review of general steps of finite ele-
ment analysis of metal structures. The chapter enables beginners to
understand the fundamentals of finite element analysis and modeling of
complicated structural behavior of metals. The chapter also includes how
to divide a metal structural element into finite elements and how to select
the best type of finite elements to represent the overall structural element.
The chapter provides a brief review of the selection of displacement func-
tions and definition of strain�displacement and stress�strain relationships.
In addition, Chapter 2 also presents a brief review of the formation of
element stiffness matrices and equations, the assemblage of these equations,
and how the assembled equations are solved for unknowns.
Chapter 3 focuses on finite element modeling of metal structures and
details the choice of element type and mesh size that can accurately simu-
late the complicated behavior of different metal structural elements. The
chapter details how the nonlinear material behavior can be efficiently
modeled and how the initial local and overall geometric imperfections
were incorporated in the finite element analysis. Chapter 3 also details
modeling of different loading and boundary conditions commonly applied
to metal structures. The chapter focuses on the finite element modeling
using any software or finite element package, as an example in this book,
the use of ABAQUS [1.27] software in finite element modeling.
2 Finite Element Analysis and Design of Metal Structures
Chapter 4 extends the information covered in Chapter 3 to explain and
detail the commonly used linear and nonlinear analyses in finite element
modeling of metal structures. The chapter also explains the analyses gener-
ally used in any software and details as an example the linear and nonlinear
analyses used by ABAQUS [1.27]. The chapter also contains a brief survey
and background of the linear and nonlinear analyses. It details the linear
eigenvalue used to model initial local and overall geometric imperfections.
The nonlinear material and geometrical analyses related to metal structures
are also highlighted in Chapter 4. In addition, the chapter also gives a
detailed explanation for the RIKS method used in ABAQUS [1.27] that
can accurately model the collapse behavior of metal structural elements.
Chapters 5�7 give illustrative examples for finite element models
developed to understand the structural behavior of metal columns, beams,
and tubular connections, respectively. These chapters start by a brief
introduction to the contents as well as a detailed review on previous
investigations on the subject. The chapters also detail the developed finite
element models and the results obtained. The presented examples show
the effectiveness of finite element models in providing detailed data that
complement experimental data in the field. The results are discussed
to show the significance of the finite element models in predicting the
structural response of different metal structural elements.
Finally, Chapter 8 presents design examples for metal tubular connec-
tions. The chapter starts by a brief introduction to the contents. The
chapter also details the finite element models developed for the presented
metal tubular connections. The design rules specified in current codes
of practice for the presented connections are also discussed and detailed
in this chapter. At the end of the chapter, comparisons between design
predictions and finite element results are presented.
1.2. TYPES OF METAL STRUCTURES
The main objective of this book is to provide a complete piece of work
regarding finite element analysis of metal structures. Hence, it is decided
to highlight finite element modeling of main metal structural elements,
which are columns, beams, and tubular connections. The metal structures
cover structures that may be constructed from any metal such as carbon
steel, cold-formed steel, stainless steel, aluminum, or any other metals.
The aforementioned materials have different stress�strain curves, yield,
and post-yield criteria. Figure 1.1 shows examples of stress�strain curves
3Introduction
for some of the aforementioned metals. For example, the stress�strain
curves of stainless steel, high strength steel, and aluminum have a rounded
behavior with no yield plateau compared with the stress�strain curves of
carbon steel as shown in Figure 1.1. Hence, the structural performance of
these metal columns, beams, and tubular connections will be different
from that of carbon steel. This book provides a detailed description on
finite element analysis of columns, beams, and tubular connections that
are composed of any metallic materials. It should also be noted that the
structural performance of different metals varies at ambient temperature
as well as at elevated temperatures. However, this book only focuses on
analyzing metal structures at ambient temperature. Furthermore, the finite
element analysis of metal structures depends on the type of applied loads.
For example, the structural performance of metal structural elements sub-
jected to static loads differs from that subjected to seismic, cyclic, dynamic
loads or any other types of loads. However, this book details the finite
element analysis of metal structures subjected to static loads or any other
loads that can be replaced by equivalent static loads.
Looking at the metal columns analyzed using the finite element
method in this book, the columns can be individual metal columns,
which represent the cases of metal column test specimens. On the other
hand, the columns investigated can be parts of structural metal frames or
trusses. The columns presented in this book can have different end
boundary conditions that vary from free to fixed-ended columns, different
lengths, and different cross sections constructed from hot-rolled, cold-
formed, or welded built-up sections. Figure 1.2 shows examples of differ-
ent column cross sections that can be investigated using finite element
Strain
S
tr
es
s
Mild steel
Austenitic stainless steel
High strength steel
Aluminum alloy
Figure 1.1 Stress�strain curves of different metals.
4 Finite Element Analysis and Design of Metal Structures
analysis covered in this book. The examples of cross sections are square,
rectangular, circular, I-shaped, solid, hollow, stiffened, and unstiffened
sections.
The metal beams presented in this book using the finite element
method can also form single metal beams such as metal beam test speci-
mens. Alternatively, the beams can be part of floor beams used in struc-
tural metal frames or framed trusses. Therefore, the beams investigated
also can have different end boundary conditions that vary from free to
fixed support with or without rigid and semi-rigid internal and end
supports. The beams investigated can have different lengths and different
Figure 1.2 Cross sections of some metal columns covered in this book.
5Introduction
cross sections constructed from hot-rolled, cold-formed, or welded built-
up sections. Figure 1.3 shows examples of different beam cross sections
that can be investigated using finite element analysis. The examples of cross
sections include I-shaped, channel, hollow, castellated, cellular, stiffened,
and unstiffened sections, as shown in Figure 1.3.
Investigating the interaction between metal columns and beams using
finite element analysis is also covered in this book. The beams and col-
umns are the main supporting elements of any metal frames and trusses.
By highlighting the structural performance of metal tubular connections,
Figure 1.3 Cross sections of some metal beams covered in this book.
6 Finite Element Analysisand Design of Metal Structures
the building structural behavior can be investigated. The connections
investigated can have different boundary conditions at the ends and can
be rigid or semi-rigid connections. The tubular connections can have
different cross sections constructed from hot-rolled, cold-formed, and
welded sections. Figure 1.4 shows examples of different tubular connec-
tions that can be investigated using finite element analysis as detailed
in this book. The tubular connections comprise square, rectangular, and
circular hollow sections.
1.3. EXPERIMENTAL INVESTIGATIONS AND ITS ROLE FOR
FINITE ELEMENT MODELING
Experimental investigation plays a major role in finite element analysis.
It is important to verify and validate the accuracy of finite element models
using test data, particularly nonlinear finite element models. In order to
Figure 1.4 Configurations of some metal tubular connections covered in this book.
7Introduction
investigate the performance of a structural member, the member must be
either tested in laboratory to observe the actual behavior or theoretically
analyzed to obtain an exact closed-form solution. Getting an exact solution
sometimes becomes very complicated and even impossible in some cases
that involve highly nonlinear material and geometry analyses. However,
experimental investigations are also costly and time consuming, which
require specialized laboratory and expensive equipment as well as highly
trained and skilled technician. Without the aforementioned requirements,
the test data and results will not be accurate and will be misleading to finite
element development. Therefore, accurate finite element models should be
validated and calibrated against accurate test results.
Experimental investigations conducted on metal structures can be
classified into full-scale and small-scale tests. In structural member tests,
full-scale tests are conducted on members that have the same dimensions,
material properties, and boundary conditions as that in actual buildings
or constructions. On the other hand, small-scale tests are conducted on
structural members that have dimensions less proportional to actual
dimensions. The full-scale tests are more accurate without the size effect
and provide more accurate data compared with small-scale tests; however,
they are more expensive in general. Most of the experimental investiga-
tions carried out on metal structures are destructive tests in nature. This is
attributed to the tests that are carried out until failure or collapse of the
member in order to predict the capacity, failure mode, and overall
structural member behavior. Tests must be very well planned and suffi-
ciently instrumented to obtain required information. Efficient testing
programs must investigate most of the parameters that affect the structural
performance of tested specimens. The programs should also include
some repeated tests to check the accuracy of the testing procedures.
Experimentalists can efficiently plan the required number of tests, position,
type, and number of instrumentations as well as significant parameters to be
investigated.
Experimental investigations on metal structures are conducted to
obtain required information from the tests using proper instrumentations
and measurement devices. Although the explanation of various instru-
mentations and devices is not in the scope of this book, the required
information for finite element analysis is highlighted herein. The required
information can be classified into three main categories: initial data, mate-
rial data, and data at the time of experiment. The initial data are obtained
from test specimens prior to testing, such as the initial local and overall
8 Finite Element Analysis and Design of Metal Structures
geometric imperfections, residual stresses, and dimensions of test speci-
mens. The material data are conducted on tensile or compression coupon
test specimens taken from untested specimens or material tests conducted
on whole untested specimens, such as stub column tests, to determine the
stress�strain curves of the materials. Knowing the stress�strain curves of
materials provide the data regarding the yield stress, ultimate stress, strain
at yield, strain at failure, ductility as well as initial modulus of elasticity.
Finally, the data at the time of experiment provide the strength of
structural test specimens, load�displacement relationships, load�strain
relationships, and failure modes. The aforementioned data are examples
of the main and commonly needed data for finite element analysis;
however, the authors of this book recommend that each experimental
investigation should be treated as an individual case and the data required
have to be carefully studied to cover all parameters related to the tested
structural element.
The tests conducted by Young and Lui [1.28,1.29] on cold-formed
high strength stainless steel square and rectangular hollow section columns
provided useful and required initial data, material data, and data at the time
of experiment for development of finite element model. First, the tests
have provided detailed data regarding initial local and overall geometric
imperfections as well as residual stresses in the specimens, which represent
“initial data.” Second, the tests have provided detailed material properties
for flat and corner portions of the sections, which represent “material
data.” Finally, the tests have provided detailed data on the compression
column tests, which represent “test data at the time of experiment.”
Figure 1.5 shows the measured membrane residual stress distributions in
cold-formed high strength stainless steel rectangular hollow section. The
values of the residual stresses that are “material data” can be incorporated
in the finite element model.
1.4. FINITE ELEMENT MODELING OF METAL STRUCTURES
Although extensive experimental investigations were presented in the
literature on metal structures, the number of tests on some research topics
is still limited. For example, up-to-date, the presented tests (Section 1.3) on
cold-formed high strength stainless steel columns carried out by Young
and Lui [1.28,1.29] remain pioneer in the field, and there is a lack of test
data that highlight different parameters outside the scope of the presented
experimental program [1.28,1.29]. The number of tests conducted on a
9Introduction
specific research topic in the field of metal structures is limited by many
factors. The factors comprise time, costs, labor, capacity of testing frame,
capacity of loading jack, measurement equipment, and testing devices.
Therefore, numerical investigations using finite element analysis were
performed and found in the literature to compensate the lack of test data
in the field of metal structures. However, detailed explanation on how
successful finite element analysis can provide a good insight into the
structural performance of metal structures was not fully addressed as a
complete piece of work, which is credited to this book.
Following experimental investigations on metal structures, finite ele-
ment analyses can be performed and verified against available test results.
Successful finite element models are those that are validated against suffi-
cient number of tests, preferably from different sources. Finite element
modeling can be extended, once validated, to conduct parametric studies
investigating the effects of the different parameters on the behavior and
strength of metal structures. The analyses performed in the parametric
studies must be well planned to predict the performance of the investi-
gated structural elements outside the ranges covered in the experimental
program. The parametric studies will generate more data that fill in the
gaps of the test results. Hence, one of the advantages of the finite element
modeling is to extrapolate the test data. However, the more significant
advantage of finite elementmodeling is to clarify and explain the test
data, which is credited to successful finite element models only. Successful
finite element models can critically analyze test results and explain reasons
150
100
50
0
Distance (mm)
–50
–100S
tr
es
s 
(M
P
a)
–150
–200
–250
Weld
100500 150 200 250 300
e
c
b
c
d eba
a
b
c
d
e
Specimen 1 (extensometer)
Specimen 2 (strain gauges)
Figure 1.5 Measured membrane residual stress distributions in cold-formed high
strength stainless steel tubular section [1.29].
10 Finite Element Analysis and Design of Metal Structures
behind failure of metal structures. The successful finite element models
can go deeply in the test results to provide deformations, stresses, and
strains at different locations in the test specimens, which is very difficult
to be determined by instrumentation. The successful finite element mod-
els can save future tests in the studied research topic owing to that they
can investigate different lengths, boundary conditions, cross sections,
geometries, material strengths, and different loading.
As an example on how finite element analysis can generate more
data to complement test results, the column tests conducted by Young
and Lui [1.28,1.29] were modeled by Ellobody and Young [1.30]. The
tested specimens were 15 square and rectangular hollow sections of
cold-formed high strength stainless steel columns. The measured initial
local and overall geometric imperfections and material nonlinearity of the
flat and corner portions of the high strength stainless steel sections were
carefully incorporated in the finite element model [1.30]. The column
strengths and failure modes as well as the load-shortening curves of the
columns were obtained using the finite element model. The validated
finite element model [1.30] was used to perform parametric studies
involving 42 new columns. The new columns investigated the effects of
cross section geometries on the strength and behavior of cold-formed
high strength stainless steel columns.
1.5. CURRENT DESIGN CODES
Design guides and specifications are proposed in different countries to
define standards of metal structural sections, classification of sections,
methods of analysis for structural members under different loading and
boundary conditions, design procedures, material strengths, and factors of
safety for designers and practitioners. The design guides are commonly
based on experimental investigations. Many design formulas specified in
current codes of practice are in the form of empirical equations proposed
by experts in the field of metal structures. However, the empirical equa-
tions only provide guidance for design of metal structural elements in the
ranges covered by the specifications. The ranges covered by the specifica-
tion depend on the number of tests conducted on the metal structural
elements at the time of proposing the codes. Since there are continuing
progress in research to discover new materials, sections, connections, and
different loading, the codes of practice need to update from time to time.
Furthermore, test programs on metal structural elements are dependent
11Introduction
on limits of the test specimens, loading, boundary conditions, and so on.
Therefore, the design equations specified in current codes of practice
always have limitations. Finite element analysis can provide a good insight
into the behavior of metal structural elements outside the ranges covered
by specifications. In addition, finite element analysis can check the valid-
ity of the empirical equations for sections affected by nonlinear material
and geometry, which may be ignored in the specifications. Furthermore,
design guides specified in current codes of practice contain some assump-
tions based on previous measurements, e.g., assuming values for initial
local and overall imperfections in metal structural elements. Also, finite
element modeling can investigate the validity of these assumptions. This
book addresses the efficiency of finite element analyses, and the numerical
results are able to improve design equations in the current codes of prac-
tice more accurately. However, it should be noted that there are many
specifications developed all over the world for metal structures, such as
steel structures, stainless steel structures, cold-formed steel structures, and
aluminum structures. It is not the intension to include all these codes of
practice in this book. Once again, this book focuses on finite element
analysis. Therefore, the book only highlights the codes of practice related
to the metal structures that performed finite element analysis.
As an example, the cold-formed high strength stainless steel columns
tested by Young and Lui [1.28,1.29] and modeled by Ellobody and
Young [1.30] as discussed in Sections 1.3 and 1.4, respectively, were
assessed against the predications by the design codes of practice related to
cold-formed stainless steel structures. The column test results [1.28,1.29]
and finite element analysis results [1.30] were compared with design
strengths calculated using the American [1.31], Australian/New Zealand
[1.32], and European [1.33] specifications for cold-formed stainless steel
structures. Based on the comparison between finite element analysis
strengths and design strengths, it was concluded [1.30] that the design
rules specified in the American, Australian/New Zealand, and European
specifications are generally conservative for cold-formed high strength
stainless steel square and rectangular hollow section columns, but uncon-
servative for some of the short columns. It should be noted that this is
an example on stainless steel columns only. The finite element analysis can
be used to other metal structures. Subsequently, more numerical data
can be generated and design equations in current codes of practice can be
improved to cope with the advances in technology, materials, and construc-
tions. Due to the advances in technology and materials, new construction
12 Finite Element Analysis and Design of Metal Structures
materials and new structural sections are being produced. For example,
a relatively new type of stainless steel called lean duplex, high strength
structural steel having yield stress of 960 MPa or above, and section shape
of oval and other shapes are used in construction.
REFERENCES
[1.1] Oden, J. T. Finite element of nonlinear continua. New York: McGraw-Hill, 1972.
[1.2] Kardestuncer, H. Elementary matrix analysis of structures. New York: McGraw-Hill,
1974.
[1.3] Whiteman, J. R. A bibliography for finite elements. London: Academic Press, 1975.
[1.4] Norrie, D. and deVries, G. Finite element bibliography. New York: IFI/Plenum, 1976.
[1.5] Zienkiewicz, O. C. The finite element method. 3rd ed., London: McGraw-Hill, 1977.
[1.6] Cook, R. D. Concepts and applications of finite element analysis. 2nd ed., New
York: John Wiley & Sons, 1981.
[1.7] Logan, H. A first course in the finite element method. Boston: PWS Engineering, 1986.
[1.8] Timoshenko, S. P. and Gere, J. M. Theory of elastic stability. New York:
McGraw-Hill, 1961.
[1.9] Bresler, B. and Lin, T. Y. Design of steel structures. New York: John Wiley & Sons,
1964.
[1.10] Case, J. and Chiler, A. H. Strength of materials. London: Edward Arnold, 1964.
[1.11] Richards, K. G. Fatigue strength of welded structures. Cambridge: The Welding
Institute, 1969.
[1.12] Boyd, G. M. Brittle fracture in steel structures. London: Butterworths, 1970.
[1.13] Steed designer manual. Crosby, Lockwood, London, 1972.
[1.14] Johnson, B. G. Guide to stability design criteria for metal structures. 3rd Ed., New
York: John Wiley & Sons, 1976.
[1.15] Trahair, N. S. The behaviour and design of steel structures. London: Chapman
and Hall, 1977.
[1.16] Ghali, A. and Neville, A. M. Structural analysis. London: Chapman and Hall,
1978.
[1.17] Pratt, J. L. Introduction of the welding of structural steelwork. London: Constrado,
1979.
[1.18] Horne,M. R. Plastic theory of structures. Oxford: Pergamon Press, 1979.
[1.19] Pask, J. W. Manual on connections for beam and column construction. London:
BCSA, 1981.
[1.20] Jenkins, V. M. Structural mechanics and analysis. New York: Van Nostrand-Reinhold,
1982.
[1.21] Holmes, M. and Martin, L. H. Analysis and design of structural connections—
reinforced concrete and steel. London: Ellis Horwood, 1983.
[1.22] Bates, W. Design of structural steelwork: Lattice framed industrial buildings.
London: Constrado, 1983.
[1.23] Steelwork design guide to BS 5950: Part I, Vol. 1, Section properties, member
capacities. The Steel Construction Institute, Ascot, 1987.
[1.24] Steelwork design guide to BS 5950: Part I, Vol. 2, Worked examples. The Steel
Construction Institute, Ascot, 1986.
[1.25] MacGinley, T. J. and Ang, T. C. Structural steelwork: Design to limit state theory.
Oxford: Butterworth-Heinemann Ltd., 1992.
[1.26] Yu, W. W. Cold-formed steel design. 3rd Edition, Inc., New York: John Wiley &
Sons, 2000.
13Introduction
http://refhub.elsevier.com/B978-0-12-416561-8.00001-9/sbref1
http://refhub.elsevier.com/B978-0-12-416561-8.00001-9/sbref2
http://refhub.elsevier.com/B978-0-12-416561-8.00001-9/sbref2
http://refhub.elsevier.com/B978-0-12-416561-8.00001-9/sbref3
http://refhub.elsevier.com/B978-0-12-416561-8.00001-9/sbref4
http://refhub.elsevier.com/B978-0-12-416561-8.00001-9/sbref5
http://refhub.elsevier.com/B978-0-12-416561-8.00001-9/sbref5
http://refhub.elsevier.com/B978-0-12-416561-8.00001-9/sbref6
http://refhub.elsevier.com/B978-0-12-416561-8.00001-9/sbref6
http://refhub.elsevier.com/B978-0-12-416561-8.00001-9/sbref6
http://refhub.elsevier.com/B978-0-12-416561-8.00001-9/sbref7
http://refhub.elsevier.com/B978-0-12-416561-8.00001-9/sbref8
http://refhub.elsevier.com/B978-0-12-416561-8.00001-9/sbref8
http://refhub.elsevier.com/B978-0-12-416561-8.00001-9/sbref9
http://refhub.elsevier.com/B978-0-12-416561-8.00001-9/sbref9
http://refhub.elsevier.com/B978-0-12-416561-8.00001-9/sbref10
http://refhub.elsevier.com/B978-0-12-416561-8.00001-9/sbref11
http://refhub.elsevier.com/B978-0-12-416561-8.00001-9/sbref11
http://refhub.elsevier.com/B978-0-12-416561-8.00001-9/sbref12
http://refhub.elsevier.com/B978-0-12-416561-8.00001-9/sbref13
http://refhub.elsevier.com/B978-0-12-416561-8.00001-9/sbref13
http://refhub.elsevier.com/B978-0-12-416561-8.00001-9/sbref13
http://refhub.elsevier.com/B978-0-12-416561-8.00001-9/sbref14
http://refhub.elsevier.com/B978-0-12-416561-8.00001-9/sbref14
http://refhub.elsevier.com/B978-0-12-416561-8.00001-9/sbref15
http://refhub.elsevier.com/B978-0-12-416561-8.00001-9/sbref15
http://refhub.elsevier.com/B978-0-12-416561-8.00001-9/sbref16
http://refhub.elsevier.com/B978-0-12-416561-8.00001-9/sbref16
http://refhub.elsevier.com/B978-0-12-416561-8.00001-9/sbref17
http://refhub.elsevier.com/B978-0-12-416561-8.00001-9/sbref18
http://refhub.elsevier.com/B978-0-12-416561-8.00001-9/sbref18
http://refhub.elsevier.com/B978-0-12-416561-8.00001-9/sbref19
http://refhub.elsevier.com/B978-0-12-416561-8.00001-9/sbref19
http://refhub.elsevier.com/B978-0-12-416561-8.00001-9/sbref20
http://refhub.elsevier.com/B978-0-12-416561-8.00001-9/sbref20
http://refhub.elsevier.com/B978-0-12-416561-8.00001-9/sbref21
http://refhub.elsevier.com/B978-0-12-416561-8.00001-9/sbref21
http://refhub.elsevier.com/B978-0-12-416561-8.00001-9/sbref22
http://refhub.elsevier.com/B978-0-12-416561-8.00001-9/sbref22
http://refhub.elsevier.com/B978-0-12-416561-8.00001-9/sbref23
http://refhub.elsevier.com/B978-0-12-416561-8.00001-9/sbref23
http://refhub.elsevier.com/B978-0-12-416561-8.00001-9/sbref23
[1.27] ABAQUS Standard User’s Manual. Hibbitt, Karlsson and Sorensen, Inc. Vol. 1, 2
and 3, Version 6.8-1, USA, 2008.
[1.28] Young, B. and Lui, W. M. Tests of cold-formed high strength stainless steel com-
pression members. Thin-walled Structures, Elsevier Science, 44(2), 224�234, 2006.
[1.29] Young, B. and Lui, W. M. Behavior of cold-formed high strength stainless steel sec-
tions. Journal of Structural Engineering, ASCE, 131(11), 1738�1745, 2005.
[1.30] Ellobody, E. and Young, B. Structural performance of cold-formed high strength
stainless steel columns. Journal of Constructional Steel Research, 61(12),
1631�1649, 2005.
[1.31] ASCE. Specification for the design of cold-formed stainless steel structural mem-
bers. Reston (VA): American Society of Civil Engineers, SEI/ASCE-02, 2002.
[1.32] AS/NZS, Cold-formed stainless steel structures. Australian/New Zealand
Standard, Sydney (Australia): Standards Australia, AS/NZS 4673:2001, 2001.
[1.33] EC3. Eurocode 3: design of steel structures—Part 1.4: General rules—
Supplementary rules for stainless steels. Brussels: European Committee for
Standardization, ENV 1993-4, CEN, 1996.
14 Finite Element Analysis and Design of Metal Structures
http://refhub.elsevier.com/B978-0-12-416561-8.00001-9/sbref24
http://refhub.elsevier.com/B978-0-12-416561-8.00001-9/sbref24
http://refhub.elsevier.com/B978-0-12-416561-8.00001-9/sbref24
http://refhub.elsevier.com/B978-0-12-416561-8.00001-9/sbref25
http://refhub.elsevier.com/B978-0-12-416561-8.00001-9/sbref25
http://refhub.elsevier.com/B978-0-12-416561-8.00001-9/sbref25
http://refhub.elsevier.com/B978-0-12-416561-8.00001-9/sbref26
http://refhub.elsevier.com/B978-0-12-416561-8.00001-9/sbref26
http://refhub.elsevier.com/B978-0-12-416561-8.00001-9/sbref26
http://refhub.elsevier.com/B978-0-12-416561-8.00001-9/sbref26
http://refhub.elsevier.com/B978-0-12-416561-8.00001-9/sbref27
http://refhub.elsevier.com/B978-0-12-416561-8.00001-9/sbref27
http://refhub.elsevier.com/B978-0-12-416561-8.00001-9/sbref28
http://refhub.elsevier.com/B978-0-12-416561-8.00001-9/sbref28
http://refhub.elsevier.com/B978-0-12-416561-8.00001-9/sbref28
CHAPTER22
Review of the General Steps of
Finite Element Analysis
2.1. GENERAL REMARKS
This chapter presents a brief review of the finite element method for
application on metal structures. The development of the finite element
method in the field of structural engineering was credited to the numeri-
cal investigations performed by Hernnikoff [2.1] and McHenery [2.2].
The investigations [2.1,2.2] were limited to the use of one-dimensional
(1D) elements for the evaluation of stresses in continuous structural
beams. The investigations [2.1,2.2] were followed by the use of shape
functions as a method to obtain approximate numerical investigations as
detailed in Ref. [2.3]. Following the study [2.3], the flexibility or force
method was proposed [2.4,2.5] mainly for analyzing aircraft structures.
Two-dimensional (2D) elements were first introduced in Ref. [2.6], where
stiffness matrices were derived for truss, beam, and 2D triangular and
rectangular elements in plane stress conditions. The study [2.6] has out-
lined the fundamentals of the stiffness method for predicting the structure
stiffness matrix. The development of the finite element method was first
introduced by Clough [2.7] where triangular and rectangular elements
were used for the analysis of structures under plane stress conditions.
In 1961, Melosh [2.8] developed the stiffness matrix for flat rectangu-
lar plate bending elements that was used for the analysis of plate struc-
tures. This was followed by developing the stiffness matrix of curved shell
elements for the analysis of shell structures as detailed by Grafton and
Strome [2.9]. Numerous investigations were developed later on to high-
light the finite element analysis of three-dimensional (3D) structures as pre-
sented in Refs [2.10�2.15]. Most of the aforementioned investigations
addressed structures under small strains and small displacements, elastic
material, and static loading. Structures that underwent large deflection
and buckling analyses were detailed in Refs [2.16,2.17], respectively.
Improved numerical techniques for the solution of finite element equa-
tions were first addressed by Belytschko [2.18,2.19]. Recent developments
15
Finite Element Analysis and Design of Metal Structures
DOI: http://dx.doi.org/10.1016/B978-0-12-416561-8.00002-0© 2014 Elsevier Inc.
All rights reserved.
http://dx.doi.org/10.1016/B978-0-12-416561-8.00002-0
in computers have resulted in the finite element method being used to
describe complicated structures associated with large number of equations.
Numerous special-purpose and general-purpose programs have been written to
analyze various complicated structures with the advent of computers and
computational programs. However, to successfully use computers in finite
element analyses, it is important to understand the fundamentals of devel-
oping finite element models comprising the definition of nodal coordinates,
finite elements and how they are connected, material properties of the
elements, applied loads, boundary conditions, and the kind of analysis to
be performed.
There are two main approaches associated with finite element analyses,
which are dependent on the type of results predicted from the analyses.
The first approach is commonly known as force or flexibility method, which
considers internal forces are the unknowns of the analyses. On the other
hand, the second approach is called the displacement or stiffness method,
which deals with nodal displacement as the unknowns of the analyses. The
finite element formulations associated with the two approaches have differ-
ent matrices that are related to flexibility or stiffness. Previous investigations
by Kardestuncer [2.20] have shown that the displacement method is more
desirable from computational purposes, and its finite element formulations,
for most of the structural analyses, are simple compared with the force
method. The majority of general-purpose finite element programs have
adopted the displacement method. Therefore, the displacement method
will be explained in this chapter. It should be noted that, in the displace-
ment method, the unknown displacements calculated during the analysis
are normally called degrees of freedom. The degrees of freedom are transla-
tional and rotational displacements at each node. The number of degrees
of freedom depends on the element type, and hence it is variable from a
structure to another.
The finite element method is based on modeling the structure using
small interconnected elements called finite elements with defined points
forming the element boundaries called nodes. There are numerous finite
elements analyzed in the literature such as bar, beam, frame, solid, and shell
elements. The use of any element depends on the type of the structure,
geometry, type of analysis, applied loads and boundary conditions, compu-
tational time, and data required from the analysis. Each element has its own
displacement function that describes the displacement within the element
in terms of nodal displacement. Every interconnected element has to be
linked to other elements simulating the structure directly by sharing the
16 Finite Element Analysis and Design of Metal Structures
exact boundaries or indirectly through the use of interface nodes, lines, or
elements that connect the element with the other elements. The element
stiffness matrices and finite element equations can be generated by making
use of the commonly known stress�strain relationships and direct equi-
librium equations. By solving the finite element equations, the unknown
displacements can be determined and used to predict different straining
actions such as internal forces and bending moments.
The main objective of this chapter is to provide a general review of the
main steps of finite element analysis of structures, specifically for metal
structures. This chapter introduces the background of the finite element
method that was used to write most of the special and general-purpose
programs available in the literature. In addition, this chapter reviews differ-
ent finite element types used to analyze metal structures. The selection of
displacement functions, definition of strain�displacement, stress�strain
relationships, the formation of element stiffness matrices and equations, the
assemblage of these equations, and how the assembled equations are solved
for unknowns are also briefed in this chapter. A simplified illustrative
example is also included in this chapter to show how these steps are
implemented. It is intended not to complicate the derived finite element
equations presented in this chapter and not to present more examples
since they are previously detailed in numerous finite element books in
the literature, with examples given in Refs [1.1�1.7].
2.2. DIVIDING AND SELECTION OF ELEMENT TYPES
FOR METAL STRUCTURES
The first step of the finite element method is to divide the structure into
small or finite elements defined by nodes located at the element edges.
The location of nodes must be chosen to define the positions of changes
in the structure. The changes comprise variation of geometry, material,
loading, and boundary conditions. The guidelines to divide or mesh dif-
ferent metal structures will be detailed in the coming chapters. It is also
important to choose the best finite elements to represent and simulate the
structure. 1D elements or bar or truss elements shown in Figure 2.1A are
often used to model metal trusses. The elements have a cross-sectional
area, which is commonly constant, but usually presented by line seg-
ments. The simplest line element has two nodes, one at each end, and is
called linear 1D element. Higher order elements are curved elements that
have three or four nodes and are called quadratic and cubic 1D elements,
17Review of the General Steps of Finite Element Analysis
respectively. The line element is the simplest form of element and there-
fore can be used to explain the basic concepts of the finite element
method in this chapter. 2D elements or plane elements shown in
Figure 2.1B are often used to model metal structures that are loaded by
forces in their own plane, commonly named as plane stress or plane strain
conditions. Plane stress elements can be used when the thickness of a metal
(A) (B)
(C)
(D) Quadratic tetrahedron Quadratic triangular prism Quadratic cubic prism
y
x
1
2
P2 P1
Cubic prism
y
x
7
5
1
3
2
4
6
8
Triangular prism
y
x
2
5
6
4
1
3
Tetrahedron
y
x
2
3
4
1
y
x1
2
3
4
5
6
7
8
9 10
11
12
13
14
15
16
17
18
19
20
y
x
1
5 6
78
9
10
2
3
4
y
x1 2
3
Triangle
Px1
Py1
Px2
Py2
Px3
Py3
y
x1 2
4 3
Quadrilateral
Px3
Py3
Px2
Py2
Px4
Py4
Px1
Py1
y
x
1
2
3
4
5
6
7 8
9
10 11
12
13
15
14
Figure 2.1 Element types commonly used in metal structures: (A) 1D (bar or truss)
element, (B) 2D (plane stress or plane strain) elements, (C) linear 3D solid elements,
and (D) quadratic 3D solid elements.
18 Finite Element Analysis and Design of Metal Structures
structure is small relative to its lateral (in-plane) dimensions. The stresses
are functions of planar coordinates alone, and the out-of-plane normal
and shear stresses are equal to zero. Plane stress elements must be defined
in the X�Y plane, and all loading and deformation are also restricted to
this plane. This modeling method generally applies to thin, flat bodies.
On the other hand, plane strain elements can be used when it can be
assumed that the strains in a loaded metal structure are functions of planar
coordinates alone and the out-of-plane normal and shear strains are equal
to zero. Plane strain elements must be defined in the X�Y plane, and all
loading and deformation are also restricted to this plane. This modeling
method is generally used for metal structures that are very thick relative
to their lateral dimensions. The main 2D elements used are triangular or
quadrilateral elements and usually have constant thickness. The simplest
2D elements have nodes at corners and are called linear 2D elements.
Higher order elements are curved sided elements that have one or two
nodes between corners and are called quadratic and cubic 2D elements,
respectively.
Finally, the 3Delements, brick, or solid elements, shown in Figure 2.1C
and D, are often used to model metal structures that are loaded by forces
in 3D named three-dimensional stress analysis. The main elements used are
tetrahedral and hexahedral elements and usually used to represent metal
structures that have complicated 3D geometry. The simplest 3D elements
have nodes at corners as shown in Figure 2.1C and are called linear 3D
elements. Higher order elements are curved surface elements that have one
or two nodes between corners as shown in Figure 2.1D and are called
quadratic and cubic 3D elements, respectively. The axisymmetric elements are
3D elements as shown in Figure 2.2 that are formed by rotating a triangle
(Figure 2.2A) or quadrilateral (Figure 2.2B) about a fixed axis throughout
360�. They are used to model metal structures that have axisymmetric
geometry. The axisymmetric elements are commonly given coordinates
using the r2 θ2 z domain, where r is the radius from origin to node,
θ is the angle from horizontal axis, and z is the vertical coordinate, as
shown in Figure 2.2.
From the structural point of view, the element types can be classified
mainly to truss, beam, frame, and shell elements. Truss or membrane
elements are elements that transmit in-plane forces only (no bending
moments) and have no bending stiffness, as shown in Figure 2.3A. The
elements are mainly long, slender structural members such as link
members and are presented in 1D. Beam elements are the elements that
19Review of the General Steps of Finite Element Analysis
transfer lateral forces and bending moments. Hence, the deformations
associated with beam elements are transverse displacement and rotation,
as shown in Figure 2.3B. The dimensions of the cross section are small
compared to the dimensions along the axis of the beam. The axial dimen-
sion must be interpreted as a global dimension (not the element length),
such as distance between supports or distance between gross changes in
cross section. The main advantage of beam elements is that they are geo-
metrically simple and have few degrees of freedom. This simplicity is
achieved by assuming that the member’s deformation can be estimated
entirely from variables that are functions of position along the beam axis
only. Frame elements are elements that provide efficient modeling for
design calculations of frame-like structures composed of initially straight,
slender members. They operate directly in terms of axial force, trans-
verse force, and bending moments at the element’s end nodes. Hence,
the deformations associated with frame elements are axial and transverse
displacements and rotation, as shown in Figure 2.3C. Frame elements
are two-node, initially straight, slender beam elements intended for use
in the analysis of frame-like structures. Similar to beam elements, frame
elements are commonly presented in 2D. However, some of the general-
purpose programs have the ability to analyze beams and frames in 3D
by including additional degrees of freedom for the elements in the plane
perpendicular to their plane.
It should be noted that the fundamental assumption used with beam
and frame elements’ section is that it cannot deform in its own plane. The
implications of this assumption should be considered carefully in any use
(A) (B)
z
r
θ
z
r
θ
Figure 2.2 Axisymmetric solid elements: (A) develop by rotating a triangle and
(B) develop by rotating a quadrilateral.
20 Finite Element Analysis and Design of Metal Structures
of beam and frame elements, especially for cases involving large amounts
of bending or axial tension/compression of non-solid cross sections such
as pipes, I-beams, and U-beams. Beam and frame elements’ section col-
lapse may occur and result in very weak behavior that is not predicted by
the assumptions of beam theory. Similarly, thin-walled, curved pipes
exhibit much softer bending behavior than would be predicted by beam
(A)
(B)
(C)
(D)
y
x1 2
y
x2
5
3
1 4
6 7y
x
21
ux2ux1
Px2Px1
vy1 vy2
1 2θ1 θ2
1
2 3
y
x
v 1
v 2 u 2
1
2
 
 
θ1
θ2
z y
x
1
2
3
4
w3
u3
v3
θx3
θy3
θz3
w4
u4
v4
θx4
θy4
θz4
w2
u2
v2
θx2
θy2
θz2
w1
u1
v1
θx1
θy1
θz1
Figure 2.3 Commonly used structural elements: (A) plane truss element, (B) plane
beam element, (C) plane frame element, and (D) shell element.
21Review of the General Steps of Finite Element Analysis
theory because the pipe wall readily bends in its own section. This effect,
which must generally be considered when designing piping elbows, can
be modeled by using shell elements. Shell elements are used to model
structures in which one dimension (the thickness) is significantly smaller
than the other dimensions. Shell elements use this condition to discretize
a structure by defining the geometry at a reference surface, commonly
the mid-plane surface. Shell elements have displacement and rotational
degrees of freedom at nodes, as shown in Figure 2.3D. The shell section
behavior may require numerical integration over the section, which can
be linear or nonlinear and can be homogeneous or composed of layers of
different material.
The number of elements required to simulate a structure is very
important. The more elements used to simulate a structure, the more
usable results we get and the more efficiency we obtain to represent the
structural behavior. However, the more elements used, the more compu-
tational time to perform the finite element analysis. It should be noted
that the increase in the number of elements does not increase the accu-
racy of the results obtained after a certain number, and any increase in the
number of the elements would give approximately the same result as
shown in Figure 2.4. Hence, the element size (number of elements) has
to be carefully decided to give accurate results compared with tests or
exact closed-form solution and at the same time to take reasonable
computational time.
No. of elements
Results
Optimum no. of elements
Exact solution
Figure 2.4 Effect of number of elements on the accuracy of results.
22 Finite Element Analysis and Design of Metal Structures
2.3. SELECTION OF A DISPLACEMENT FUNCTION
After dividing the structure into suitable finite elements, a displacement
function or a shape function within each element has to be chosen. As
mentioned previously, each element type has a certain function that is
characteristic to this element. For example, a displacement function for 1D
elements is not suitable to represent 2D or 3D elements. The displacement
function is defined as the function that describes the displacement within
the element in terms of the nodal values of the element. The functions that
can be used as shape functions are polynomial functions and may be linear,
quadratic, or cubic polynomials. However, trigonometric series can be also
used as shape functions. For example, the displacement function of a
2D element is a function of the coordinates in its plane (X�Y plane).
The functions are expressed in terms of the nodal unknowns (an x and a
y component). The same displacement function can be used to describe
the displacement behavior within each of the remaining finite elements of
the structure. Hence, the finite element method treats the displacement
throughout the whole structure approximately as a discrete model com-
posed of a set of piecewise continuous functions defined within each finite
element of the structure.
2.4. DEFINITION OF THE STRAIN�DISPLACEMENT AND
STRESS�STRAIN RELATIONSHIPS
The next step, following the selection of a displacement function, is to
define the strain�displacement and stress�strain relationships. The relation-
ships depend on the element type and are used to derive the governing
equations of each finite element. As an example, a 1D finite element
has only one deformation along the axis of the element (x-direction in
Figure 2.1A. Assuming that the axial displacement is u, then the axialstrain
associated with this deformation εx can be evaluated as follows:
εx 5
du
dx
ð2:1Þ
To evaluate the stresses in the element, the stress�strain relationship
or constitutive law has to be used. The relationship is also characteristic
to the element type and in this simple 1D finite element, Hooke’s law
23Review of the General Steps of Finite Element Analysis
can be applied to govern the stress�strain relationship throughout the
element as follows:
σx5Eεx ð2:2Þ
where σx is the stress in direction x, which is related to the strain εx, and
E is the modulus of elasticity.
2.5. DERIVATION OF THE ELEMENT STIFFNESS MATRIX
AND EQUATIONS
The next step, following the definition of strain�displacement and
stress�strain relationships, is to derive the element stiffness matrix and
equations that relate nodal forces to nodal displacements. The element
stiffness matrix depends on the element type and it is characteristic to the
element. The element matrices are commonly developed using direct equi-
librium method and work or energy methods. The direct equilibrium method
is the simplest approach to derive the stiffness matrix and element equa-
tions. The method is based on applying force equilibrium conditions and
force�deformation relationships for each finite element. This method is
easy to apply for 1D finite elements and becomes mathematically tedious
for higher order elements. Therefore, for 2D and 3D finite elements, the
work method is easier to apply. The work method is based on the princi-
ple of virtual work as detailed in Ref. [2.21]. Both the direct equilibrium
and work methods will yield the same finite element equations relating
the nodal forces with nodal displacements as follows:
ff g5 ½k�fdg ð2:3Þ
where ff g is the vector of nodal forces, [k] is the finite element stiffness
matrix, and {d} is the vector of unknown finite element nodal degrees of
freedom or displacements. The formulation of the aforementioned finite
element matrices will be explained in this chapter by an illustrative exam-
ple for 1D finite elements. Similar approach can be used for any other
elements as detailed in Refs [1.1�1.7].
2.6. ASSEMBLAGE OF ELEMENT EQUATIONS
Following the derivation of the individual element stiffness matrix and
equations of each finite element of the structure, the global stiffness matrix
and equation of the whole structure can be assembled. The assemblage of
24 Finite Element Analysis and Design of Metal Structures
the global stiffness matrix and equation is generated by adding and
superimposing the individual matrices and equations using the direct stiffness
method, which is based on the equilibrium of nodal forces. The direct
stiffness method is based on the fact that, for any structure in equilibrium,
the nodal forces and displacements must be in continuity and compatibility
in the individual finite element as well as in the whole structure. The global
finite element equation can be expressed in matrix form as follows:
fFg5 ½K �fdg ð2:4Þ
where {F} is the assembled vector of the whole structure global nodal forces,
[K] is the whole structure assembled global stiffness matrix, and {d} is the
assembled vector of the whole structure global unknown nodal degrees
of freedom or displacements. It should be noted that Eq. (2.4) must be
modified to account for the boundary conditions or support constraints.
The modification will be explained in the illustrative example detailed in this
chapter. Also, it should be noted that Eq. (2.3) may be evaluated for each
finite element with respect to local coordinate system. However, the assem-
bled equation (2.4) must be evaluated with respect to a unique generalized
coordinate system. Hence, transformation matrices must be used to relate local
coordinates to general coordinate systems, as detailed in Refs [1.1�1.7].
2.7. SOLVING THE ASSEMBLED EQUATIONS
FOR THE UNKNOWNS
Solving Eq. (2.4) will result in the evaluation of the unknown nodal
degrees of freedom or generalized displacements. The equation can be
solved using algebraic procedures such as elimination or iterative methods
detailed in Refs [1.1�1.7]. The calculated unknown nodal degrees of
freedom (translational displacements and rotations) can be used to evaluate
all required variables in the structure such as stresses, strains, bending
moments, shear forces, axial forces, and reactions. The evaluation of
the aforementioned variables can be used to design the structure and
to define its failure modes and positions of maximum and minimum
deformations and stresses.
2.7.1 An Illustrative Example
The metal structure shown in Figure 2.5A is a structural bar (fixed free-
edged structure) having linear elastic material properties, two equal length
parts (L15L25L) of different cross-sectional areas (A1 and A2) and
25Review of the General Steps of Finite Element Analysis
different moduli of elasticity (E1 and E2). The structural bar is loaded at
its free edge with a load P3. At the first step, the bar is divided into two
elements (1�2 and 2�3). The nodes defining the elements (1, 2, and 3) are
located at the positions of the change in boundary conditions, geometry and
loading, respectively. As a revision, the previously detailed Refs [1.1�1.7]
derivation of the finite element equations governing a single finite element
1�2, shown in Figure 2.5B, can be summarized in the following sections.
To represent the deformations within the 1D finite element 1�2 in terms of
nodal displacement, a linear polynomial shape function can be expressed as
in Eq. (2.5):
u5 a11 a2x ð2:5Þ
where u is the axial deformation in x-direction, a1 and a2 are coefficients
that are equal to the number of degrees of freedom, 2 for this 1D element.
To express the function u in terms of nodal displacements d1x and d2x,
we can solve Eq. (2.5) to obtain the equation coefficients as follows:
At x5 0.0, u5 d1x, and by substituting in Eq. (2.5), a15 d1x.
(A)
(B)
Given: A1 = 200 mm2; A2 = 100 mm2; P3 = 10 N; 
 L1 = L2 = 100 mm; E1 = E2 = 2 × 105MPa
1
y
x
2 3
P3
A1, E1 A2, E2
1
y
x
2 3
d3xd2xd1x
L1 L2
1
y
d1x
x
2
f1x = –F f2x = F
d2x
A1 = A
L1 = L
Figure 2.5 Finite element analysis of a structural bar: (A) structural bar and (B) finite
element 1�2.
26 Finite Element Analysis and Design of Metal Structures
Also, at x5L, u25 d2x and once again by substituting in Eq. (2.5),
d2x5 d1x1 a2L and a25 ðd2x2 d1xÞ=L. By substituting the values of a1
and a2 in Eq. (2.5), we can express the deformations within element 1�2
in terms of nodal displacements at nodes 1 and 2 as in Eq. (2.6):
u5 d1x1 ðd2x 2 d1xÞx=L ð2:6Þ
To derive the element stiffness matrix, we have to define the
strain�displacement and stress�strain relationships. The axial strain (εx)
for this 1D element can be expressed as the difference between nodal dis-
placement divided by the element length L as in Eq. (2.7).
εx 5
du
dx
5 ðd2x2 d1xÞ=L ð2:7Þ
Now, we can use Hooke’s law to govern the stress�strain relationship
throughout the element as expressed in Eq. (2.8):
σx5Eεx ð2:8Þ
where, σxis the axial stress and E is Young’s modulus.
The nodal forces can be now calculated by multiplying the cross-
sectional area A by the axial stress σx and substituting the axial strain from
Eq. (2.7) as in Eq. (2.9):
F5Aσx5AEεx5
EA
L
ðd2x2 d1xÞ ð2:9Þ
We can now write the nodal force equations by assuming a sign conven-
tion that the force at node 1 ( f1x) is equal to 2F and that at node 2 ( f2x) is
equal to F. By substituting the nodal forces in Eq. (2.9), we can write the
nodal forces f1x and f2x as follows:
f1x5
EA
L
ðd1x2 d2xÞ ð2:10Þ
f2x5
EA
L
ðd2x2 d1xÞ ð2:11Þ
Equations (2.10 and 2.11) can be written in matrix form as in
Eq. (2.12) and in a compact form as expressed in Eq. (2.13).
f1x
f2x
� �
5
EA
L
1 21
21 1
� �
d1x
d2x
� �
5
k11 k12
k21 k22
� �
d1x
d2x
� �
ð2:12Þ
27Review of the General Steps of Finite Element Analysis
f
� �
5 k½ � df g ð2:13Þ
We can noweasily analyze the structural bar as shown in Figure 2.5A
given that the cross-sectional areas A1 and A2 are 200 and 100 mm2,
respectively, the moduli of elasticityE15E2 5E5 23 105 N=mm2, the
force P3 is equal to 10 N, and finally the lengths L15L25L5 100 mm.
The stiffness matrices for finite elements 1�2 and 2�3 ([k12] and [k23])
can be evaluated as follows:
k12½ �5E1A1
L1
1 21
21 1
� �
5
200;0003200
100
1 21
21 1
� �
5105
4 24
24 4
� �
5
k11 k12
k21 k22
� �
k23½ �5E2A2
L2
1 21
21 1
� �
5
200;0003100
100
1 21
21 1
� �
5105
2 22
22 2
� �
5
k22 k23
k32 k33
� �
The two stiffness matrices [k12] and [k23] can now be assembled to
form the global stiffness matrix of the structural bar [K] noting that there
are the stiffness k13 and k31 as follows:
½K�5
k11 k12 k13
k21 k221k22 k23
k31 k32 k33
2
4
3
55 k11 k12 0
k21 k221k22 k23
0 k32 k33
2
4
3
55105
4 24 0
24 6 22
0 22 2
2
4
3
5
The global force vector fFg and displacement vector fdg can now be
written as follows:
fFg5
f1x
f2x
f3x
8<
:
9=
;5
R1
0
10
8<
:
9=
;
fdg5
d1x
d2x
d3x
8<
:
9=
;5
0
d2x
d3x
8<
:
9=
;
The finite element governing equation of the structural bar can now be
written and solved for unknown displacements (d2x and d3x) as follows:
R1
0
10
8<
:
9=
;5 105
4 24 0
24 6 22
0 22 2
2
4
3
5 0
d2x
d3x
8<
:
9=
;
28 Finite Element Analysis and Design of Metal Structures
0
10
� �
5 105
6 22
22 2
� �
d2x
d3x
� �
05 105ð6d2x2 2d3xÞ ‘3d2x5 d3x
105 105ð2 2d2x1 2d3xÞ ‘105 105ð2 2d2x1 6d2xÞ
‘d2x5 2:53 1025 mm and d3x5 7:53 1025 mm
We can now obtain all required information regarding the structural
bar such as unknown reaction R1, element strains, and stresses as follows:
R15 1053 ð2 4Þ3 d2x5 1053 ð2 4Þ3 2:53 102552 10 N
ε1x5
d2x2 d1x
L1
5
2:53 10252 0
100
5 2:53 1027
ε2x5
d3x2 d2x
L2
5
7:53 10252 2:53 1025
100
5 53 1027
σ1x 5E1ε1x5 23 1053 2:53 10275 0:05 N=mm2
σ2x5E2ε2x5 23 1053 53 10275 0:1 N=mm2
The same approach used to analyze 1D truss elements can be used to
analyze beam, frame, shell, and solid structural elements as detailed in
Refs [1.1�1.7]. The finite element equations and matrices of these
elements will become more complicated as the number of degrees of
freedom increases. Also, solving the finite element governing equations
of higher order elements and obtaining unknown reactions, element
strains and element stresses will be more complicated. However, these
complicated equations and its solving techniques have been very easy
nowadays because of the advances in computers.
29Review of the General Steps of Finite Element Analysis
REFERENCES
[2.1] Hrennikoff, A. Solution of problems in elasticity by the frame work method.
Journal of Applied Mechanics, 8(4), 169�175, 1941.
[2.2] McHenry, D. A lattice analogy for the solution of plane stress problems. Journal of
Institution of Civil Engineers, 21, 59�82, 1943.
[2.3] Courant, R. Variational methods for the solution of problems of equilibrium and
vibrations. Bulletin of the American Mathematical Society, 49, 1�23, 1943.
[2.4] Levy, S. Computation of influence coefficients for aircraft structures with disconti-
nuities and sweepback. Journal of Aeronautical Sciences, 14(10), 547�560, 1947.
[2.5] Levy, S. Computation of influence coefficients for delta wings. Journal of
Aeronautical Sciences, 20(7), 449�454, 1953.
[2.6] Turner, M. G., Clough, R. W., Martin, H. C. and Topp, L. J. Stiffness and deflec-
tion analysis of complex structures. Journal of Aeronautical Sciences, 23(9),
805�824, 1956.
[2.7] Clough, R. W. The finite element method in plane stress analysis. Proceedings of
American Society of Civil Engineers, 2nd Conference on Electronic computation,
Pittsburg, Pa., 345�378, 1960.
[2.8] Melosh, R. J. A stiffness matrix for the analysis of thin plates in bending. Journal
of Aerospace Sciences, 28(1), 34�42, 1961.
[2.9] Grafton, P. E. and Strome, D. R. Analysis of axisymmetric shells by the direct stiff-
ness method. Journal of the American Institute of Aeronautics and Astronautics,
1(10), 2342�2347, 1963.
[2.10] Martin, H. C. Plane elasticity problems and the direct stiffness method. The Trend
in Engineering, 13, 5�19, 1961.
[2.11] Gallagher, R. H., Padlog, J. and Bijlaard, P. P. Stress analysis of heated complex
shapes. Journal of the American Rocket Society, 32, 700�707, 1962.
[2.12] Melosh, R. J. Structural analysis of solids. Journal of the Structural Division,
Proceedings of the American Society of Civil Engineers, 205�223, 1963.
[2.13] Argyris, J. H. Recent advances in matrix methods of structural analysis. Progress
in Aeronautical Sciences, 4, New York: Pergamon Press, 1964.
[2.14] Clough, R. W. and Rashid, Y. Finite element analysis of axisymmetric solids.
Journal of the Engineering Mechanics Division, Proceedings of the American
Society of Civil Engineers, 91, 71�85, 1965.
[2.15] Wilson, E. L. Structural analysis of axisymmetric solids. Journal of the American
Institute of Aeronautics and Astronautics, 3(12), 2269�2274, 1965.
[2.16] Turner, M. G., Dill, E. H., Martin, H. C. and Melosh, R. J. Large deflections of
structures subjected to heating and external loads. Journal of Aeronautical
Sciences, 27(2), 97�107, 1963.
[2.17] Gallagher, R. H. and Padlog, J. Discrete element approach to structural stability
analysis. Journal of the American Institute of Aeronautics and Astronautics, 1(6),
1437�1439, 1963.
[2.18] Belytschko, T. A survey of numerical methods and computer programs for
dynamic structural analysis. Nuclear Engineering and Design, 37(1), 23�34, 1976.
[2.19] Belytschko, T. Efficient large-scale nonlinear transient analysis by finite elements.
International Journal of Numerical Methods in Engineering, 10(3), 579�596, 1981.
[2.20] Kardestuncer, H. Elementary matrix analysis of structures. New York: McGraw-Hill,
1974.
[2.21] Oden, J. T. and Ripperger, E. A. Mechanics of elastic structures. New York:
McGraw-Hill, 1981.
30 Finite Element Analysis and Design of Metal Structures
http://refhub.elsevier.com/B978-0-12-416561-8.00002-0/sbref1
http://refhub.elsevier.com/B978-0-12-416561-8.00002-0/sbref1
http://refhub.elsevier.com/B978-0-12-416561-8.00002-0/sbref1
http://refhub.elsevier.com/B978-0-12-416561-8.00002-0/sbref2
http://refhub.elsevier.com/B978-0-12-416561-8.00002-0/sbref2
http://refhub.elsevier.com/B978-0-12-416561-8.00002-0/sbref2
http://refhub.elsevier.com/B978-0-12-416561-8.00002-0/sbref3
http://refhub.elsevier.com/B978-0-12-416561-8.00002-0/sbref3
http://refhub.elsevier.com/B978-0-12-416561-8.00002-0/sbref3
http://refhub.elsevier.com/B978-0-12-416561-8.00002-0/sbref4
http://refhub.elsevier.com/B978-0-12-416561-8.00002-0/sbref4
http://refhub.elsevier.com/B978-0-12-416561-8.00002-0/sbref4
http://refhub.elsevier.com/B978-0-12-416561-8.00002-0/sbref5
http://refhub.elsevier.com/B978-0-12-416561-8.00002-0/sbref5
http://refhub.elsevier.com/B978-0-12-416561-8.00002-0/sbref5
http://refhub.elsevier.com/B978-0-12-416561-8.00002-0/sbref6
http://refhub.elsevier.com/B978-0-12-416561-8.00002-0/sbref6
http://refhub.elsevier.com/B978-0-12-416561-8.00002-0/sbref6
http://refhub.elsevier.com/B978-0-12-416561-8.00002-0/sbref6
http://refhub.elsevier.com/B978-0-12-416561-8.00002-0/sbref7
http://refhub.elsevier.com/B978-0-12-416561-8.00002-0/sbref7
http://refhub.elsevier.com/B978-0-12-416561-8.00002-0/sbref7
http://refhub.elsevier.com/B978-0-12-416561-8.00002-0/sbref8
http://refhub.elsevier.com/B978-0-12-416561-8.00002-0/sbref8
http://refhub.elsevier.com/B978-0-12-416561-8.00002-0/sbref8
http://refhub.elsevier.com/B978-0-12-416561-8.00002-0/sbref8
http://refhub.elsevier.com/B978-0-12-416561-8.00002-0/sbref9
http://refhub.elsevier.com/B978-0-12-416561-8.00002-0/sbref9
http://refhub.elsevier.com/B978-0-12-416561-8.00002-0/sbref9
http://refhub.elsevier.com/B978-0-12-416561-8.00002-0/sbref10
http://refhub.elsevier.com/B978-0-12-416561-8.00002-0/sbref10
http://refhub.elsevier.com/B978-0-12-416561-8.00002-0/sbref10
http://refhub.elsevier.com/B978-0-12-416561-8.00002-0/sbref11
http://refhub.elsevier.com/B978-0-12-416561-8.00002-0/sbref11http://refhub.elsevier.com/B978-0-12-416561-8.00002-0/sbref11
http://refhub.elsevier.com/B978-0-12-416561-8.00002-0/sbref12
http://refhub.elsevier.com/B978-0-12-416561-8.00002-0/sbref12
http://refhub.elsevier.com/B978-0-12-416561-8.00002-0/sbref13
http://refhub.elsevier.com/B978-0-12-416561-8.00002-0/sbref13
http://refhub.elsevier.com/B978-0-12-416561-8.00002-0/sbref13
http://refhub.elsevier.com/B978-0-12-416561-8.00002-0/sbref13
http://refhub.elsevier.com/B978-0-12-416561-8.00002-0/sbref14
http://refhub.elsevier.com/B978-0-12-416561-8.00002-0/sbref14
http://refhub.elsevier.com/B978-0-12-416561-8.00002-0/sbref14
http://refhub.elsevier.com/B978-0-12-416561-8.00002-0/sbref15
http://refhub.elsevier.com/B978-0-12-416561-8.00002-0/sbref15
http://refhub.elsevier.com/B978-0-12-416561-8.00002-0/sbref15
http://refhub.elsevier.com/B978-0-12-416561-8.00002-0/sbref15
http://refhub.elsevier.com/B978-0-12-416561-8.00002-0/sbref16
http://refhub.elsevier.com/B978-0-12-416561-8.00002-0/sbref16
http://refhub.elsevier.com/B978-0-12-416561-8.00002-0/sbref16
http://refhub.elsevier.com/B978-0-12-416561-8.00002-0/sbref16
http://refhub.elsevier.com/B978-0-12-416561-8.00002-0/sbref17
http://refhub.elsevier.com/B978-0-12-416561-8.00002-0/sbref17
http://refhub.elsevier.com/B978-0-12-416561-8.00002-0/sbref17
http://refhub.elsevier.com/B978-0-12-416561-8.00002-0/sbref18
http://refhub.elsevier.com/B978-0-12-416561-8.00002-0/sbref18
http://refhub.elsevier.com/B978-0-12-416561-8.00002-0/sbref18
http://refhub.elsevier.com/B978-0-12-416561-8.00002-0/sbref19
http://refhub.elsevier.com/B978-0-12-416561-8.00002-0/sbref19
http://refhub.elsevier.com/B978-0-12-416561-8.00002-0/sbref20
http://refhub.elsevier.com/B978-0-12-416561-8.00002-0/sbref20
CHAPTER33
Finite Element Modeling
3.1. GENERAL REMARKS
The brief revision of the finite element method is presented in Chapter 2.
It is now possible to detail the main parameters affecting finite element
modeling and simulation of different metal structural members, which is
highlighted in this chapter. The chapter provides useful guidelines on how to
choose the best finite element type and mesh to represent metal columns,
beams and beam columns, and connections. The behavior of different finite
elements, briefed in Chapter 2, is analyzed in this chapter to assess their
suitability for simulating the structural member. There are many parameters
that control the choice of finite element type and mesh such as the geometry,
cross section classification, loading, and boundary conditions of the structural
member. The aforementioned issues are also covered in this chapter.
Accurate finite element modeling depends on the efficiency in simulating the
nonlinear material behavior of metal structural members. This chapter shows
how to correctly represent different linear and nonlinear regions in the
stress�strain curves of metal structures. Most of metal structures have initial
local and overall geometric imperfections as well as residual stresses as a result
of the manufacturing process. Ignoring the simulation of these initial imper-
fections and residual stresses would result in poor finite element models that
are unable to describe the performance of the metal structure. The correct
simulation of different initial geometric imperfections and residual stresses
is also addressed in this chapter. In addition, there are different loads and
boundary conditions applied to metal columns, beams and beam columns,
and connections. Improper simulation of applied loads and boundary
conditions on a structural member would not provide an accurate finite
element model. Therefore, correct simulation of different loads and
boundary conditions that are commonly associated with metal structural
members is highlighted in this chapter. Furthermore, the chapter presents
examples of finite element models developed in the literature and
successfully simulated the performance of different structures. It should
be noted that the sections described in this chapter detail the finite
element modeling using any software and any finite element package.
31
Finite Element Analysis and Design of Metal Structures
DOI: http://dx.doi.org/10.1016/B978-0-12-416561-8.00003-2
© 2014 Elsevier Inc.
All rights reserved.
http://dx.doi.org/10.1016/B978-0-12-416561-8.00003-2
However, as an example, the use of ABAQUS software [1.27] to simulate
different metal structures is detailed in this chapter.
3.2. CHOICE OF ELEMENT TYPE FOR METAL STRUCTURES
To explain how to choose the best finite element type to simulate the
behavior of a metal structure, let us start with modeling a stainless steel
column having a rectangular hollow section as shown in Figure 3.1. The
first step is to look into the classification of the cross section that is nor-
mally specified in all current codes of practice. There are three commonly
known cross section classifications that are compact, noncompact, and
slender sections. Compact sections have a thick plate thickness and can
develop their plastic moment resistance without the occurrence of local
buckling. Noncompact sections are sections in which the stress in the
extreme fibers can reach the yield stress, but local buckling is liable to
prevent development of the plastic moment resistance. Finally, slender
sections are those sections in which local buckling will occur in one or
more parts of the cross section before reaching the yield strength.
Compact sections in 3D can be modeled either using solid elements or
Stainless steel tube
(B)
D
B
t
ri
d
S S
(A)
L
(C)
Given: 
L=1400 mm, D=160 mm,
B=80 mm, t=3 mm,
ri=6.3 mm
Figure 3.1 Example of a fixed-ended rectangular hollow section column. (A) Fixed-
ended rectangular hollow section column. (B) Rectangular hollow section (section S-S).
(C) Finite element mesh.
32 Finite Element Analysis and Design of Metal Structures
shell elements that are able to model thick sections. However, noncom-
pact and slender sections are only modeled using shell elements that are
able to model thin sections. It should be noted that many general-
purpose programs have shell elements that are used to simulate thin and
thick sections. Finite element models are normally developed to perform
different analyses and parametric studies on different cross sections; hence,
it is recommended to choose shell elements in modeling the rectangular
hollow section column as shown in Figure 3.1.
Let us take a look in detail and classify shell elements commonly used
in modeling structural members. There are two main shell element cate-
gories known as conventional and continuum shell elements, examples shown
in Figure 3.2. Conventional shell elements cover elements used for 3D shell
geometries, elements used for axisymmetric geometries, and elements
used for stress�displacement analysis. The conventional shell elements
can be classified as thick shell elements, thin shell elements, and general-
purpose shell elements that can be used for the analysis of thick or thin
shells. Conventional shell elements have six degrees of freedom per node;
however, it is possible to have shells with five degrees of freedom per
node. Numerical integration is normally used to predict the behavior
within the shell element. Conventional shell elements can use full or
(B)
(A)
1
2
S3 shell element S4 shell element S8 shell element
3
1 2
4 3
4 3
1 2
8
7
5
6
Wedge element Hexahedron element
3
6
2
5
1
4
4
1
3
2
7
6
5
8
Figure 3.2 Shell element types: (A) conventional shell elements and (B) continuum
shell elements.
33Finite Element Modeling
reduced numerical integration, as shown in Figure 3.3. Reduced integration
shell elements use lower order integration to form the element stiffness.
However, the mass matrix and distributed loadings are still integrated
exactly. Reduced integration usually provides accurate results provided
that the elements are not distorted or loaded in in-plane bending.
Reduced integrationsignificantly reduces running time, especially in
three dimensions. Shell elements are commonly identified based on the
number of element nodes and the integration type. Hence, a shell ele-
ment S8 means a stress�displacement shell having eight nodes with full
integration while a shell element S8R means a stress�displacement shell
having eight nodes with reduced integration. On the other hand, contin-
uum shell elements are general-purpose shells that allow finite membrane
deformation and large rotations and, thus, are suitable for nonlinear geo-
metric analysis. These elements include the effects of transverse shear
deformation and thickness change. Continuum shell elements employ
first-order layer-wise composite theory and estimate through-thickness
section forces from the initial elastic moduli. Unlike conventional shells,
continuum shell elements can be stacked to provide more refined
through-thickness response. Stacking continuum shell elements allows for
a richer transverse shear stress and force prediction. It should be noted
(A)
(B)
S3
1 2
4
3 4 3
1 2
8
7
5
6
1 2
3
S4 S8
3
1 2
3
4
1 2
374
8 6
1 5 2
S3R
1 2
4
3 4 3
1 2
8
7
5
6
1 2
3
SR4 S8R
34
1 21
1
Figure 3.3 Full and reduced integration of shell elements: (A) full integration and (B)
reduced integration.
34 Finite Element Analysis and Design of Metal Structures
that most metal structures are modeled using conventional shell elements
and hence they are detailed in this book.
General-purpose conventional shell elements allow transverse shear
deformation. They use thick shell theory as the shell thickness increases
and become discrete Kirchhoff thin shell elements as the thickness
decreases. The transverse shear deformation becomes very small as the
shell thickness decreases. Examples of these elements are S3, S3R, S4,
and S4R shells. Thick shells are needed in cases where transverse shear
flexibility is important and second-order interpolation is desired. When a
shell is made of the same material throughout its thickness, this occurs
when the thickness is more than about 1/15 of a characteristic length on
the surface of the shell, such as the distance between supports. An exam-
ple of thick elements is S8R. Thin shells are needed in cases where trans-
verse shear flexibility is negligible and the Kirchhoff constraint must be
satisfied accurately (i.e., the shell normal remains orthogonal to the shell
reference surface). For homogeneous shells, this occurs when the
thickness is less than about 1/15 of a characteristic length on the surface
of the shell, such as the distance between supports. However, the thick-
ness may be larger than 1/15 of the element length.
Conventional shell elements can also be classified as finite-strain and
small-strain shell elements. Element types S3, S3R, S4, and S4R account for
finite membrane strains and arbitrarily large rotations; therefore, they are
suitable for large-strain analysis. On the other hand, small-strain shell
elements such as S8R shell elements are used for arbitrarily large rotations
but only small strains. The change in thickness with deformation is
ignored in these elements. For conventional shell elements used in
ABAQUS [1.27], we must specify a section Poisson’s ratio as part of the
shell section definition to allow for the shell thickness in finite-strain ele-
ments to change as a function of the membrane strain. If the section
Poisson’s ratio is defined as zero, the shell thickness will remain constant
and the elements are, therefore, suited for small-strain, large-rotation anal-
ysis. The change in thickness is ignored for the small-strain shell elements
in ABAQUS [1.27].
Conventional reduced integration shell elements can be also classified
based on the number of degrees of freedom per node. Hence, there are
two types of conventional reduced integration shell elements known as
five-degrees and six-degrees of freedom shells. Five-degrees of freedom con-
ventional shells have five degrees of freedom per node, which are three
translational displacement components and two in-plane rotation
35Finite Element Modeling
components. On the other hand, six-degrees of freedom shells have six
degrees of freedom per node, which are three translational displacement
components and three rotation components. The number of degrees
of freedom per node is commonly denoted in the shell name by adding
digit 5 or 6 at the end of the reduced integration shell element name.
Therefore, reduced integration shell elements S4R5 and S4R6 have five
and six degrees of freedom per node, respectively. The elements that use
five degrees of freedom per node such as (S4R5 and S8R5) can be more
economical. However, they are suitable only for thin shells and they can-
not be used for thick shells. The elements that use five degrees of free-
dom per node cannot be used for finite-strain applications, although they
model large rotations with small strains accurately.
There are a number of issues that must be considered when using shell
elements. Both S3 and S3R refer to the same three-node triangular shell
element. This element is a degenerated version of S4R that is fully com-
patible with S4 and S4R elements. S3 and S3R provide accurate results
in most loading situations. However, because of their constant bending
and membrane strain approximations, high mesh refinement may be
required to capture pure bending deformations or solutions to problems
involving high strain gradients. Curved elements such as S8R5 shell
elements are preferable for modeling bending of a thin curved shell.
Element type S8R5 may give inaccurate results for buckling problems of
doubly curved shells due to the fact that the internally defined integration
point may not be positioned on the actual shell surface. Element type S4
is a fully integrated, general-purpose, finite-membrane-strain shell element.
Element type S4 has four integration locations per element compared with
one integration location for S4R, which makes the element computation
more expensive. S4 is compatible with both S4R and S3R. S4 can be used
in areas where greater solution accuracy is required, or for problems where
in-plane bending is expected. In all of these situations, S4 will outperform
element type S4R.
Based on the previous survey of conventional shell elements, we can
find that the general-purpose conventional shell elements S4/S4R can be
used effectively to model a metal column having a hollow section. The
S3/S3R can also be used in combination with the S4/S4R shells to
model curved corners of the hollow section. The elements can be used
to model different compact, noncompact, and slender cross sections.
Figure 3.1 shows the finite element mesh with shell elements used by
Ellobody and Young [1.30] for a fixed-ended rectangular hollow section
36 Finite Element Analysis and Design of Metal Structures
column having a length (L) of 1400 mm, a depth (D) of 160 mm, a width
(B) of 80 mm, plate thickness (t) of 3 mm, and internal corner radius (ri)
of 6.3 mm. The authors have used S4R elements to model the flat and
curved portions of the whole column.
As mentioned earlier, metal structures that are composed of compact
sections can be modeled using solid elements. Solid or continuum ele-
ments are volume elements that do not include structural elements such
as beams, shells, and trusses. The elements can be composed of a single
homogeneous material or can include several layers of different materials
for the analysis of laminated composite solids. The naming conventions
for solid elements depend on the element dimensionality, number of
nodes in the element, and integration type. For example, C3D8R
elements are continuum elements (C), 3D elements having eight nodes
with reduced integration (R). Solid elements provide accurate results
if not distorted, particularly for quadrilaterals and hexahedra, as shown in
Figure 2.1. The triangularand tetrahedral elements are less sensitive to
distortion. Solid elements can be used for linear analysis and for complex
nonlinear analyses involving stress, plasticity, and large deformations. Solid
element library includes first-order (linear) interpolation elements and
second-order (quadratic) interpolation elements commonly in three
dimensions. Tetrahedral, triangular prisms, and hexahedra (bricks) are
very common 3D elements, as shown in Figure 2.1. Modified second-
order triangular and tetrahedral elements as well as reduced integration
solid elements can be also used. First-order plane strain, axisymmetric
quadrilateral, and hexahedral solid elements provide constant volumetric
strain throughout the element, whereas second-order elements provide
higher accuracy than first-order elements for smooth problems that do
not involve severe element distortions. They capture stress concentrations
more effectively and are better for modeling geometric features. They
can model a curved surface with fewer elements. Finally, second-order
elements are very effective in bending-dominated problems. First-order
triangular and tetrahedral elements should be avoided as much as possible
in stress analysis problems; the elements are overly stiff and exhibit slow
convergence with mesh refinement, which is especially a problem with
first-order tetrahedral elements. If they are required, an extremely fine
mesh may be needed to obtain results with sufficient accuracy.
Similar to the behavior of shells, reduced integration can be used with
solid elements to form the element stiffness. The mass matrix and distrib-
uted loadings use full integration. Reduced integration reduces running
37Finite Element Modeling
time, especially in 3D. For example, element type C3D20 has 27 integra-
tion points, while C3D20R has 8 integration points only. Therefore,
element assembly is approximately 3.5 times more costly for C3D20
than for C3D20R. Second-order reduced integration elements generally
provide accurate results than the corresponding fully integrated elements.
However, for first-order elements, the accuracy achieved with full versus
reduced integration is largely dependent on the nature of the problem.
Triangular and tetrahedral elements are geometrically flexible and can be
used in many models. It is very convenient to mesh a complex shape
with triangular or tetrahedral elements. A good mesh of hexahedral
elements usually provides a solution with equivalent accuracy at less cost.
Quadrilateral and hexahedral elements have a better convergence rate
than triangular and tetrahedral elements. However, triangular and tetrahe-
dral elements are less sensitive to initial element shape, whereas first-order
quadrilateral and hexahedral elements perform better if their shape is
approximately rectangular. First-order triangular and tetrahedral elements
are usually overly stiff, and fine meshes are required to obtain accurate
results. For stress�displacement analyses, the first-order tetrahedral
element C3D4 is a constant stress tetrahedron, which should be avoided
as much as possible. The element exhibits slow convergence with mesh
refinement. This element provides accurate results only in general cases
with very fine meshing. Therefore, C3D4 is recommended only for
filling in regions of low stress gradient to replace the C3D8 or C3D8R
elements, when the geometry precludes the use of C3D8 or C3D8R ele-
ments throughout the model. For tetrahedral element meshes, the
second-order or the modified tetrahedral elements such as C3D10 should
be used. Similarly, the linear version of the wedge element C3D6 should
generally be used only when necessary to complete a mesh, and, even
then, the element should be far from any area where accurate results are
needed. This element provides accurate results only with very fine mesh-
ing. A solid section definition is used to define the section properties of
solid elements. A material definition must be defined with the solid sec-
tion definition, which is assigned to a region in the finite element model.
As mentioned previously in Chapter 2, plane-stress and plane-strain
structures can be modeled using 2D solid elements. The naming conven-
tions for the elements depend on the element type (PE or PS) for (plane
strain or plane stress), respectively, and number of nodes in the element.
For example, CPE3 elements are continuum (C), plane strain (PE) linear
elements having three nodes, as shown in Figure 2.1. The elements have
38 Finite Element Analysis and Design of Metal Structures
two active degrees of freedom per node in the element plane. Quadratic
2D elements are suitable for curved geometry of structures. Structural
metallic link members and metallic truss members can be modeled using
1D solid elements. The naming conventions for 1D solid elements
depend on the number of nodes in the element. For example C1D3
elements are continuum (C) elements having three nodes. The elements
have one active degree of freedom per node.
Axisymmetric solid elements are 3D elements that are used to model
metal structures that have axisymmetric geometry. The element nodes are
commonly using cylindrical coordinates (r, θ, z), where r is the radius from
origin (coordinate 1), θ is the angle in degrees measured from horizontal
axis (coordinate 2), and z is the perpendicular dimension (coordinate 3) as
shown in Figure 3.4. Coordinate 1 must be greater than or equal to zero.
Degree of freedom 1 is the translational displacement along the radius (ur),
and degree of freedom 2 is the translational displacement along the perpen-
dicular direction (uz). The naming conventions for axisymmetric solid
elements with nonlinear asymmetric deformation depend on the number
z (r, θ, z)
θ
Angle in degrees
y
z
x
r
Figure 3.4 Cylindrical coordinates for axisymmetric solid elements.
39Finite Element Modeling
of nodes in the element and integration type. For example, CAXA8R ele-
ments are continuum (C) elements, axisymmetric solid elements with non-
linear asymmetric deformation (AXA) having eight nodes with reduced
(R) integration as shown in Figure 3.5. Stress�displacement axisymmetric
solid elements without twist have two active degrees of freedom per node.
3.3. CHOICE OF FINITE ELEMENT MESH
FOR METAL STRUCTURES
After choosing the best finite element type to model a metal structural
member, we need to look into the geometry of the metal structural
member to decide the best finite element mesh. Normally, most cold-
formed and hot-rolled metal structural members have flat and curved
regions. Therefore, the finite element mesh has to cover both flat and
curved regions. Also, most metal structural members have short dimen-
sions, which are commonly the lateral dimensions of the cross section,
and long dimensions, which are the longitudinal axial dimension of the
structural member that defines the structural member length. Therefore,
the finite element mesh has to cover both lateral and longitudinal regions
of the structural member. Once again, let us mesh the cold-formed stain-
less steel hollow section column shown in Figure 3.1. We have already
explained that general-purpose conventional quadrilateral shell elements
S4R can be used to model the hollow section column effectively as used
by Ellobody and Young [1.30]. To mesh the column (Figure 3.1)
correctly, we have to start with a short dimension for the chosen shell
element and decide the best aspect ratio. The aspect ratio is defined as the
x
z
y
4
2
3
1
5
6
7
8
Figure 3.5 CAXA8R axisymmetric solid elements.
40 Finite Element Analysis and Design of Metal Structures
ratio of the longest dimension to the shortest dimension of a quadrilateral
finite element. As the aspect ratio is increased, the accuracy of the results
is decreased. The aspect ratio should be kept approximately constant for
all finite element analyses performed on the column. Therefore, mostgeneral-purpose finite element software specify a maximum value for the
aspect ratio that should not be exceeded; otherwise, the results will be
inaccurate. Figure 3.6 presents a schematic diagram showing the effect of
aspect ratio on the accuracy of results. The best aspect ratio is 1, and the
maximum value, as an example the value recommended by ABAQUS
[1.27], is 5. It should be noted that the smaller the aspect ratio, the larger
the number of elements and the longer the computational time. Hence,
it is recommended to start with an aspect ratio of 1 and mesh the whole
column and compare the numerical results against test results or exact
closed-form solutions. Then we can repeat the procedure using aspect
ratios of 2 and 3 and plot the three numerical results against test results
or exact solutions. After that, we can go back and choose different short
dimensions smaller or larger than that initially chosen for the shell finite
element and repeat the aforementioned procedures and again plot the results
against test results or exact closed-form solutions. Plotting the results will
determine the best finite element mesh that provides accurate results with
less computational time. The studies we conduct to choose the best finite
element mesh are commonly called as convergence studies. It should be noted
that in regions of the structural member where the stress gradient is small,
aspect ratios higher than 5 can be used and still can produce satisfactory
0 1 2 3 4 5 6 7 8
Aspect ratio
A
cc
ur
ac
y 
of
 r
es
ul
ts
Exact solution
Nonlinear relationship
Figure 3.6 Effect of aspect ratio of finite elements on the accuracy of results.
41Finite Element Modeling
results. Figure 3.1 shows the finite element mesh used by Ellobody and
Young [1.30] to simulate the behavior of fixed-ended rectangular hollow
section columns. As mentioned by Ellobody and Young [1.30], “In order to
choose the finite element mesh that provides accurate results with minimum
computational time, convergence studies were conducted. It is found that
the mesh size of 20 mm3 10 mm (length by width) provides adequate
accuracy and minimum computational time in modeling the flat portions
of cold-formed high strength stainless steel columns, while a finer mesh was
used at the corners.”
Metal structural members having cross sections that are symmetric
about one or two axes can be modeled by cutting half or quarter of the
member, respectively, owing to symmetry. Use of symmetry reduces the
size of the finite element mesh considerably and consequently reduces
the computational time significantly. Detailed discussions on how sym-
metry can be efficiently used in finite element modeling are presented
in Ref. [3.1]. However, researchers and modelers have to be very careful
when using symmetry to reduce the mesh size of metal structural
members. This is attributed to the fact that most metal columns, beams
and beam columns, and connections that have slender cross sections can
fail owing to local buckling or local yielding. Failure due to local buckling
or local yielding can occur in any region of the metal structural member
due to initial local and overall geometric imperfections. Therefore, the
whole structural members have to be modeled even if the cross section
is symmetric about the two axes. In addition, symmetries have to be in
loading, boundary conditions, geometry, and materials. If the cross section
is symmetric but the structural member is subjected to different loading
along the length of the member or the boundary conditions are not the
same at both ends, the whole structural members have to be modeled too.
Therefore, it is better to define symmetry in this book as correspondence
in size, shape, position of loads, material properties, boundary conditions,
residual stresses due to processing, initial local, and overall geometric
imperfections that are on opposite sides of a dividing line or plane. As an
example, a tensile coupon test specimen can be modeled by considering
symmetry, as shown in Figure 3.7. The specimen is an example of a
plane-stress uniaxially loaded structure that can be modeled by using
triangular and quadrilateral plane-stress solid elements. It can be seen
that only quarter of the specimen was modeled due to symmetry. All
nodes at symmetry surfaces (1) and (2) were prevented to displace in
x-direction and y-direction, respectively. All nodes at the corner location
42 Finite Element Analysis and Design of Metal Structures
were prevented to displace in x and y-directions. It can also be seen that
the mesh is fine at the middle and curved portions of the tensile coupon
specimen where stresses are concentrated. The finite element mesh can
be coarser at ends where the specimen is fitted in the grips of the tensile
testing machine.
It should be noted that most current efficient general-purpose finite
element software have the ability to perform meshing of the metal struc-
tures automatically. However, in many cases, the resulting finite element
meshes may be very fine so that it takes huge time in the analysis process.
Therefore, it is recommended in this book to use guided meshing where
the modelers apply the aforementioned fundamentals in building the
finite element mesh using current software. In this case, automatic mesh-
ing software can be of great benefit for modelers.
3.4. MATERIAL MODELING
Most metal structures have nonlinear stress�strain curves or linear�nonlinear
stress�strain curves, as shown in Figure 1.1. The stress�strain curves can be
determined from tensile coupon tests or stub column tests specified in most
current international specifications. The stress�strain curves are characteristic
10 107.51.25 1.25
5
R=1.25
Symmetry surface (1)
Symmetry surface (2)
P (N/mm) P (N/mm)
(A)
(B)
Symmetry surface (1)
Corner
x
y
Symmetry surface 2
Figure 3.7 Use of symmetry to reduce the size of finite element meshes. (A) Plane-
stress uniaxially loaded tensile coupon test specimen. (B) Finite element mesh of
quarter of the specimen.
43Finite Element Modeling
to the construction materials and differ considerably from a material to
another. Although the testing procedures of tensile coupon tests and stub
column tests are outside the scope of this book, it is important in this chapter
to detail how the linear and nonlinear regions of the stress�strain curves are
incorporated in the finite element models. The test stress�strain curves
obtained from tensile coupon tests are commonly measured with load being
applied at a specified loading rate during different time range, which can
result in a dynamic stress�strain curve shown in Figure 3.8. The figure was
used as an example by Zhu and Young [3.2] in modeling cold-formed steel
oval hollow section columns. The nominal (engineering) static stress�strain
curve needed for finite element modeling can be obtained from a tensile
coupon test by pausing the applied straining for specified few minutes
near the proportional limit stress, the yield stress, the ultimate tensile
stress, and the post-ultimate tensile stress. This is intended to allow stress
relaxation associated with plastic straining to take place. The nominal
(engineering) static stress�strain curve is also shown in Figure 3.8. The
main important parameters needed from the stress�strain curve are the
measured initial Young’s modulus (E0), the measured proportional limit
stress (σp), the measured static yield stress (σy) that is commonly taken as
the 0.1% or 0.2% proof stress (σ0.1 or σ0.2) for materials having a rounded
stress�strain curve with no distinct yield plateau, the measured ultimate
tensile strength (σu), and the measured elongation after fracture (εf).
It should be noted that buckling analysis of metal columns, beams and
beam columns, and connections commonly involve large inelastic strains.
Therefore, the nominal (engineering) static stress�strain curves must be
converted to truestress�logarithmic plastic true strain curves. The true
500
400
300
200
100
0
0 5 10 15
Strain ε (%)
S
tr
es
s 
σ 
(M
P
a)
20 25 30
Test curve
True curve
Engineering curve
Figure 3.8 Modeling of metal plasticity [3.2].
44 Finite Element Analysis and Design of Metal Structures
stress (σtrue) and plastic true strain (εpltrue) were calculated using Eqs (3.1)
and (3.2) as given in ABAQUS [1.27]:
σtrue5σð11 εÞ ð3:1Þ
εpltrue5 lnð11 εÞ2σtrue=E0 ð3:2Þ
where E0 is the initial Young’s modulus, σ and ε are the measured nominal
(engineering) stress and strain values, respectively. Figure 3.8 also shows the
true stress-plastic true strain curve calculated using Eqs (3.1) and (3.2).
The initial part of the stress�strain curve from origin to the propor-
tional limit stress can be represented based on linear elastic model as given
in ABAQUS [1.27]. The linear elastic model can define isotropic, ortho-
tropic, or anisotropic material behavior and is valid for small elastic strains
(normally less than 5%). Depending on the number of symmetry planes
for the elastic properties, a material can be classified as either isotropic
(an infinite number of symmetry planes passing through every point) or
anisotropic (no symmetry planes). Some materials have a restricted number
of symmetry planes passing through every point; for example, orthotropic
materials have two orthogonal symmetry planes for the elastic properties.
The number of independent components of the elasticity tensor depends
on such symmetry properties. The simplest form of linear elasticity is the
isotropic case. The elastic properties are completely defined by giving the
Young’s modulus (E0) and the Poisson’s ratio (ν). The shear modulus (G)
can be expressed in terms of E0. Values of Poisson’s ratio approaching 0.5
result in nearly incompressible behavior.
The nonlinear part of the curve passing the proportional limit stress
can be represented based on classical plasticity model as given in ABAQUS
[1.27]. The model allows the input of a nonlinear curve by giving tabular
values of stresses and strains. When performing an elastic�plastic analy-
sis at finite strains, it is assumed that the plastic strains dominate the
deformation and that the elastic strains are small. It is justified because
most materials have a well-defined yield stress that is a very small per-
centage of their Young’s modulus. For example, the yield stress of most
metals is typically less than 1% of the Young’s modulus of the materials.
Therefore, the elastic strains will also be less than this percentage, and
the elastic response of the materials can be modeled quite accurately as
being linear.
45Finite Element Modeling
The classical metal plasticity models use Mises or Hill yield surfaces
with associated plastic flow, which allow for isotropic and anisotropic
yield, respectively. The models assume perfect plasticity or isotropic hard-
ening behavior. Perfect plasticity means that the yield stress does not
change with plastic strain. Isotropic hardening means that the yield surface
changes size uniformly in all directions such that the yield stress increases
(or decreases) in all stress directions as plastic straining occurs. Associated
plastic flow means that as the material yields, the inelastic deformation
rate is in the direction of the normal to the yield surface (the plastic
deformation is volume invariant). This assumption is generally acceptable for
most calculations with metal. The classical metal plasticity models can be
used in any procedure that uses elements with displacement degrees
of freedom. The Mises and Hill yield surfaces assume that yielding of
the metal is independent of the equivalent pressure stress. The Mises yield
surface is used to define isotropic yielding. It is defined by giving the value
of the uniaxial yield stress as a function of uniaxial equivalent plastic strain
as mentioned previously. The Hill yield surface allows anisotropic yielding
to be modeled.
3.5. MODELING OF INITIAL IMPERFECTIONS
Most hot-rolled and cold-formed metal structural members have initial
geometric imperfections as a result of the manufacturing, transporting,
and handling processes. Initial geometric imperfections can be classified
into two main categories, which are local and overall (bow, global, or
out-of-straightness) imperfections. Initial local geometric imperfections
can be found in any region of the outer or inner surfaces of metal
structural members and are in the perpendicular directions to the struc-
tural member surfaces. On the other hand, initial overall geometric
imperfections are global profiles for the whole structural member along
the member length in any direction. Many experimental investigations
were presented in the literature highlighting the measurement proce-
dures of initial local and overall geometric imperfections for different
structural members, which are outside the scope of this book. However,
this book details how the magnitude and profile of initial local and
overall geometric imperfections are incorporated in the finite element
models. Initial local and overall geometric imperfections can be pre-
dicted from finite element models by conducting eigenvalue buckling
analysis to obtain the worst cases of local and overall buckling modes.
46 Finite Element Analysis and Design of Metal Structures
These local and overall buckling modes can be then factored by mea-
sured magnitudes in the tests. Superposition can be used to predict final
combined local and overall buckling modes. The resulting combined
buckling modes can be then added to the initial coordinates of the
structural member. The final coordinates can be used in any subsequent
nonlinear analysis. The details of the eigenvalue buckling analysis will be
highlighted in Chapter 4.
Accurate finite element models must incorporate initial local and
overall geometric imperfections in the analysis; otherwise, the results
will not be accurate. Even in most axially loaded metal long column
tests, the columns tend to buckle in the direction of the maximum ini-
tial overall geometric imperfection. In addition, in most eccentrically
loaded metal long column tests, the initial overall geometric imperfec-
tion must be added to the eccentricity to obtain the moment resistance
of the column. Efficient test programs must include the measurement of
initial local and overall geometric imperfections. Figure 3.9 shows the
measured initial local geometric imperfection profile of stainless steel
rectangular hollow section 2003 1103 4 mm as detailed by Young and
Lui [1.29]. Table 3.1 shows the measured initial overall geometric
imperfections at mid-length of stainless steel columns as detailed by
Young and Lui [1.28].
–0.4
–0.2
0
0.2
0.4
0.6
0.8
1.2
0 100 200 300 400 500 600
Location (mm)
Im
pe
rf
ec
tio
n 
(m
m
)
A
B
C
a b c d e f g h
O
ut
si
de
In
si
de
1.0
Weld
Max. imperfection = 1.084mm
Weld
d c
b
af
e
hg
Figure 3.9 Measured local geometric imperfection profiles of RHS 2003 1103 4 [1.29].
47Finite Element Modeling
3.6. MODELING OF RESIDUAL STRESSES
Residual stresses are initial stresses existing in cross sections without
application of an external load such as stresses resulting from
manufacturing processes of metal structural members by cold forming.
Residual stresses produce internal membrane forces and bending
moments, which are in equilibrium inside the cross sections. The force
and the moment resulting from residual stresses in the cross sections
must be zero. Residual stresses in structural cross sections are attributed
to the uneven cooling of parts of cross sections after hot rolling. Uneven
cooling of cross-sectional parts subjects to internal stresses. The parts that
cool quicker have residual compressive stresses, while parts that cool lower
have residual tensile stresses. Residual stresses cannot be avoided and in
most cases are not desirable.The measurement of residual stresses is there-
fore important for accurate understanding of the performance of metal
structural members.
Table 3.1 Measured Overall Geometric Imperfections
at Mid-Length of Columns [1.28]
Specimen
δ/L
x y
SHS1L650 1/430 1/17060
SHS1L1000 1/19685 1/2386
SHS1L1500 1/11811 1/29528
SHS1L2000 1/10499 1/8288
SHS1L2500 1/29528 1/2140
SHS1L3000 1/1390 1/11811
SHS2L650 1/2326 1/4653
SHS2L1000 1/1358 1/2316
SHS2L1500 1/2953 1/1790
SHS2L2000 1/4632 1/1500
SHS2L2500 1/775 1/3076
SHS2L3000 1/872 1/993
RHS1L600 � 1/4295
RHS1L1400 � 1/7349
RHS1L2200 � 1/5588
RHS1L3000 � 1/3236
RHS2L600 � 1/7874
RHS2L1400 � 1/5512
RHS2L2200 � 1/6663
RHS2L3000 � 1/3937
48 Finite Element Analysis and Design of Metal Structures
Extensive experimental investigations were conducted in the literature
to determine the distribution and magnitude of residual stresses inside
cross sections. The experimental investigations can be classified into two
main categories: nondestructive and destructive methods. Examples of
nondestructive methods are X-ray diffraction and neutron diffraction.
Nondestructive methods are suitable for measuring stresses close to the
outside surface of cross sections. On the other hand, destructive methods
involve machining/cutting of the cross section to release internal stresses
and measure resulting change of strains. Destructive methods are based on
the destruction of the state of equilibrium of the residual stresses in the
cross section. In this way, the residual stresses can be measured by relaxing
these stresses. However, it is only possible to measure the consequences
of the stress relaxation rather than the relaxation itself. One of the main
destructive methods is to cut the cross section into slices and measure the
change in strains before and after cutting. After measuring the strains,
some simple analytical approaches can be used to evaluate resultant mem-
brane forces and bending moments in the cross sections. Although the
testing procedures to determine residual stresses are outside the scope of
this book, it is important to detail how to incorporate residual stresses in
finite element models. It should be noted that in some cases, incorporat-
ing residual stresses can result in small effect on the structural performance
of metals. However, in some other cases, it may result in considerable
effect. Since the main objective of this book is to accurately model all
parameters affecting the behavior and design of metal structures, the way
to model residual stresses is highlighted in this book.
Experimental investigations for measuring residual stresses are costly
and time consuming. Therefore, some numerical methods were presented
in the literature to simulate some typical and simple procedures introduc-
ing residual stresses. Dixit and Dixit [3.3] modeled cold rolling for steel
and gave a simplified approach to find the longitudinal residual stress. The
numerical simulation [3.3] has provided the scope to investigate the
effects of different parameters on the magnitude and distribution of resid-
ual stresses such as material characteristics and boundary conditions.
Kamamato et al. [3.4] have analyzed residual stresses and distortion of
large steel shafts due to quenching. The results showed that residual stres-
ses are strongly related to the transformational behavior. Toparli and
Aksoy [3.5] analyzed residual stresses during water quenching of cylindri-
cal solid steel bars of various diameters by using finite element technique.
The authors have computed the transient temperature distribution for
49Finite Element Modeling
solid bars with general surface heat transfer. Jahanian [3.6] modeled heat
treatment and calculated the residual stress in a long solid cylinder by
using theoretical and numerical methods with different cooling speeds.
Yuan and Wu [3.7] used a finite element program to analyze the transient
temperature and residual stress fields for a metal specimen during quench-
ing. They modified the elastic�plastic properties of specimen according
to temperature fields. Yamada [3.8] presented a method of solving
uncoupled quasi-static thermoplastic problems in perforated plates. In
their analysis, a transient thermal stress problem was solved for an infinite
plate containing two elliptic holes with prescribed temperature. In all
these models, many assumptions were made to simplify the actual process.
This is attributed to the fact that it is quite complicated to simulate all the
parameters in detail. However, reasonably good models were developed
in these pervious investigations by considering the key factors that affect
the formation of residual stresses. An extensive survey of the aforemen-
tioned numerical investigations was presented by Ding [3.9].
Residual stresses and their distribution are very important factors
affecting the strength of axially loaded metal structures. These stresses are
of particular importance for slender columns, with slenderness ratio vary-
ing from approximately 40 to 120. As a column load is increased, some
parts of the column will quickly reach the yield stress and go into the
plastic range because of the presence of residual compression stresses. The
stiffness will reduce and become a function of the part of the cross section
that is still inelastic. A column with residual stresses will behave as though
it has a reduced cross section. This reduced cross section or elastic portion
of the column will change as the applied load changes. The buckling
analysis and post-buckling calculation can be carried out theoretically or
numerically by using an effective moment of inertia of the elastic portion
of the cross section or by using the tangent modulus. ABAQUS [1.27] is
a popular package that can be used for the post-buckling analysis, which
gives the history of deflection versus loading. The ultimate strength of the
column could be then obtained from this history.
As mentioned previously in Section 1.3 of the book, efficient experi-
mental programs should measure residual stresses in tested specimens,
which are detailed as an example in the investigation conducted by
Young and Lui [1.28,1.29]. The investigation measured the residual stres-
ses in stainless steel square and rectangular hollow sections. Measurement
of residual stresses was carried out using the method of sectioning that
requires cutting the hollow section into strips to release the internal
50 Finite Element Analysis and Design of Metal Structures
residual stresses. The strains before and after cutting were measured by
the authors [1.28,1.29]; consequently, residual stresses can be determined.
The stainless steel hollow section specimens were marked into strips with
an assumed width. A gauge length was marked on the outside and inside
mid-surfaces of each strip along the length. The residual strains were
measured using an extensometer over the gauge length. The initial read-
ings before cutting were recorded for each strip together with the corre-
sponding temperature. The cutting was carried out using a wire-cutting
method in the water to eliminate additional stresses resulting from the
cutting process. The readings were taken after cutting and the corre-
sponding temperature was recorded. The readings were corrected for
temperature difference before and after cutting. The residual strains were
measured for both inner and outer sides of each strip. The membrane
residual strain was calculated as the mean of the strains, (inner strain1 outer
strain)/2. The bending strain was calculated as the difference between
the outer and inner strains divided by two, (inner strain2 outer strain)/2.
A compressive strain (negative value) was recorded at the corner, while a
tensile strain (positive value) was recorded at the flat portion. Positive
bending strain indicates compressive strain at the inner fiber and tensile
strain at the outer fiber. Residual stressesare calculated by multiplying
residual strains by Young’s modulus of the test specimens. The distribu-
tion of membrane and bending residual stresses in the cross section of the
test specimen was detailed in [1.28,1.29].
To ensure accurate modeling of the behavior of metal structures, the
residual stresses should be included in the finite element models. As an
example, the column tests conducted by Young and Lui [1.28,1.29]
were modeled by Ellobody and Young [1.30]. Measured residual stresses
were implemented in the finite element model as initial stresses using
ABAQUS [1.27] software. It should be noted that the slices cut from
the cross section to measure the residual stresses can be used to form
tensile coupon test specimens. In this case, the effect of bending stresses
on the stress�strain curve of the metal material will be considered since
the tensile coupon specimen will be tested in the actual bending condition.
Therefore, only the membrane residual stresses have to be incorporated
in the finite element model as given in Ref. [1.30]. The average values
of the measured membrane residual stresses were calculated for corner and
flat portions of the section. Figure 1.5 showed an example of the measured
membrane residual stresses conducted by Young and Lui [1.28,1.29]
and modeled by Ellobody and Young [1.30].
51Finite Element Modeling
Initial conditions can be specified for particular nodes or elements, as
appropriate. The data can be provided directly in an external input file or
in some cases by a user subroutine or by the results or output database file
from a previous analysis. If initial conditions are not specified, all initial
conditions are considered zero in the model. Various types of initial con-
ditions can be specified, depending on the analysis to be performed;
however, the type highlighted here is the initial conditions (stresses). The
option can be used to apply stresses in different directions. When initial
stresses are given, the initial stress state may not be an exact equilibrium
state for the finite element model. Therefore, an initial step should be
included to check for equilibrium and iterate, if necessary, to achieve
equilibrium.
3.7. LOAD APPLICATION
Loads applied on metal structural members in tests or in practice must be
simulated accurately in finite element models. Any assumptions or simpli-
fications in actual loads could affect the accuracy of results. There are two
common load types applied to metal structural members, which are
widely known as concentrated loads and distributed loads. Concentrated forces
and moments can be applied to any node in the finite element model.
Concentrated forces and moments are incorporated in the finite element
model by specifying nodes, associated degrees of freedom, and magnitude
and direction of applied concentrated forces and moments. The concen-
trated forces and moments could be fixed in direction or alternative can
rotate as the node rotates. On the other hand, distributed loads can be
prescribed on element faces to simulate surface distributed loads. The
application of distributed loads must be incorporated in the finite element
model very carefully using appropriate distributed load type that is
suitable to each element type. Most software specify different distributed
load types associated with the different element types included in the soft-
ware element library. For example, solid brick elements C3D8 can accept
distributed loads on eight surfaces, while shell elements are commonly
loaded in planes perpendicular to the shell element mid-surface. Distributed
loads can be defined as element-based or surface-based. Element-based distrib-
uted loads can be prescribed on element bodies, element surfaces, or element
edges. The surface-based distributed loads can be prescribed directly on
geometric surfaces or geometric edges.
52 Finite Element Analysis and Design of Metal Structures
Three types of distributed loads can be defined in ABAQUS [1.27],
which are body, surface, and edge loads. Distributed body loads are always
element-based. Distributed surface loads and distributed edge loads
can be element-based or surface-based. Body loads, such as gravity, are
applied as element-based loads. The units of body forces are force per
unit volume. Body forces can be specified on any elements in the global
x-, y-, or z-direction. Also, body forces can be specified on axisymmetric
elements in the radial or axial direction. General or shear surface tractions
and pressure loads can be applied as element-based or surface-based dis-
tributed loads. The units of these loads are force per unit area. Distributed
edge tractions (general, shear, normal, or transverse) and edge moments can
be applied to shell elements as element-based or surface-based distributed
loads. The units of edge tractions are force per unit length. The units of edge
moments are torque per unit length. Distributed line loads can be applied
to beam elements as element-based distributed loads. The units of line loads
are force per unit length. It should be noted that in some cases, distributed
surface loads can be transferred to equivalent concentrated nodal loads and
can provide reasonable accuracy provided that a fine mesh has been used.
3.8. BOUNDARY CONDITIONS
Following the load application on the finite element model, we can now
apply the boundary conditions on the finite element model. Boundary con-
ditions are used in finite element models to specify the values of all basic
solution variables such as displacements and rotations at nodes. Boundary
conditions can be given as model input data to define zero-valued boundary
conditions and can be given as history input data to add, modify, or remove
zero-valued or nonzero boundary conditions. Boundary conditions can be
specified using either direct format or type format. The type format is a way of
conveniently specifying common types of boundary conditions in
stress�displacement analyses. Direct format must be used in all other analysis
types. For both direct and type format, the region of the model to which the
boundary conditions apply and the degrees of freedom to be restrained must
be specified. Boundary conditions prescribed as model data can be modified
or removed during analysis steps. In the direct format, the degrees of free-
dom can be constrained directly in the finite element model by specifying
the node number or node set and the degree of freedom to be constrained.
As an example in ABAQUS [1.27], when you specify that (CORNER, 1),
this means that the node set named (CORNER) are constrained to displace
53Finite Element Modeling
in direction 1 (ux). While specifying that (CORNER, 1, 4), this means that
the node set CORNER are constrained to displace in directions 1�4
(ux, uy, uz, and θx). The type of boundary condition can be specified instead
of degrees of freedom. As examples in ABAQUS [1.27], specifying
“XSYMM” means symmetry about a plane X5 constant, which implies
that the degrees of freedom 1, 5, and 6 equal to 0. Similarly, specifying
“YSYMM” means symmetry about a plane Y5 constant, which implies that
the degrees of freedom 2, 4, and 6 equal to 0, and specifying “ZSYMM”
means symmetry about a plane Z5 constant, which implies that the degrees
of freedom 3, 4, and 5 equal to 0. Also, specifying “ENCASTRE” means fully
built-in (fixed case), which implies that the degrees of freedom 1, 2, 3, 4, 5,
and 6 equal to 0. Finally, specifying “PINNED” means pin-ended case, which
implies that the degrees of freedom 1, 2, and 3 equal to 0. Looking again to
Figure 3.7, we can now apply a boundary condition of type “XSYMM” to all
nodes on symmetry surface (2), and “YSYMM” can be applied to all nodes
on symmetry surface (1). It should be noted that once a degree of freedom
has been constrained using a type boundary condition as model data, the
constraint cannot be modified by using a boundary conditionin direct format
as model data. Also, a displacement-type boundary condition can be used to
apply a prescribed displacement magnitude to a degree of freedom.
The application of boundary conditions is very important in finite ele-
ment modeling. The application must be identical to the actual situation
in the metal structural member test or construction. Otherwise, the finite
element model will never produce accurate results. Modelers must be
very careful in applying all boundary conditions related to the structure
and must check that they have not overconstrained the model. Symmetry
surfaces also require careful treatment to adjust the boundary conditions
at the surface. It should be also noted that applying a boundary condition
at a node to constrain this node from displacing or rotating will totally
stop this node to displace or rotate. When the displacement or rotation is
not completely constrained (partial constraint), springs must be used to
apply the boundary conditions with constraint values depending on the
stiffness related to the degrees of freedom.
REFERENCES
[3.1] Bowes, W. H. and Russell, L. T. Stress analysis by the finite element method for prac-
ticing engineers. Toronto: Lexington Books, 1975.
[3.2] Zhu, J. H. and Young, B. Design of cold-formed steel oval hollow section columns.
Journal of Constructional Steel Research, 71, 26�37, 2012.
54 Finite Element Analysis and Design of Metal Structures
http://refhub.elsevier.com/B978-0-12-416561-8.00003-2/sbref1
http://refhub.elsevier.com/B978-0-12-416561-8.00003-2/sbref1
http://refhub.elsevier.com/B978-0-12-416561-8.00003-2/sbref2
http://refhub.elsevier.com/B978-0-12-416561-8.00003-2/sbref2
http://refhub.elsevier.com/B978-0-12-416561-8.00003-2/sbref2
[3.3] Dixit, U. S. and Dixit, P. M. A study on residual stresses in rolling. International
Journal of Machine Tools and Manufacture, 37(6), 837�853, 1997.
[3.4] Kamamato, S., Nihimori, T. and Kinoshita, S. Analysis of residual stress and distor-
tion resulting from quenching in large low-alloy steel shafts. Journal of Materials
Sciences and Technology, 1, 798�804, 1985.
[3.5] Toparli, M. and Aksoy, T. Calculation of residual stresses in cylindrical steel bars
quenched in water from 600�C, Proceedings of AMSE Conference, vol. 4, New
Delhi, India, 93�104, 1991.
[3.6] Jahanian, S. Residual and thermo-elasto-plastic stress distributions in a heat treated
solid cylinder. Materials at High Temperatures, 13(2), 103�110, 1995.
[3.7] Yuan, F. R. and Wu, S. L. Transient-temperature and residual-stress fields in axisym-
metric metal components after hardening. Journal of Materials Science and
Technology, 1, 851�856, 1985.
[3.8] Yamada, K. Transient thermal stresses in an infinite plate with two elliptic holes.
Journal of Thermal Stresses, 11, 367�379, 1988.
[3.9] Y. Ding, Residual stresses in hot-rolled solid round steel bars and their effect on
the compressive resistance of members. Master Thesis. Windsor (Ontanio, Canada):
University of Windsor, 2000.
55Finite Element Modeling
http://refhub.elsevier.com/B978-0-12-416561-8.00003-2/sbref3
http://refhub.elsevier.com/B978-0-12-416561-8.00003-2/sbref3
http://refhub.elsevier.com/B978-0-12-416561-8.00003-2/sbref3
http://refhub.elsevier.com/B978-0-12-416561-8.00003-2/sbref4
http://refhub.elsevier.com/B978-0-12-416561-8.00003-2/sbref4
http://refhub.elsevier.com/B978-0-12-416561-8.00003-2/sbref4
http://refhub.elsevier.com/B978-0-12-416561-8.00003-2/sbref4
http://refhub.elsevier.com/B978-0-12-416561-8.00003-2/sbref5
http://refhub.elsevier.com/B978-0-12-416561-8.00003-2/sbref5
http://refhub.elsevier.com/B978-0-12-416561-8.00003-2/sbref5
http://refhub.elsevier.com/B978-0-12-416561-8.00003-2/sbref6
http://refhub.elsevier.com/B978-0-12-416561-8.00003-2/sbref6
http://refhub.elsevier.com/B978-0-12-416561-8.00003-2/sbref6
http://refhub.elsevier.com/B978-0-12-416561-8.00003-2/sbref6
http://refhub.elsevier.com/B978-0-12-416561-8.00003-2/sbref7
http://refhub.elsevier.com/B978-0-12-416561-8.00003-2/sbref7
http://refhub.elsevier.com/B978-0-12-416561-8.00003-2/sbref7
CHAPTER44
Linear and Nonlinear Finite
Element Analyses
4.1. GENERAL REMARKS
The previous chapter highlighted the main parameters that control finite ele-
ment modeling of metal structures, and we can now address different linear
and nonlinear finite element analyses. This chapter presents the main analy-
ses associated with finite element modeling of metal columns and beams.
When the finite element method was introduced in Chapter 2, with a solved
example presented in Section 2.7, it was assumed that the displacements
of the finite element model are infinitesimally small and that the material is
linearly elastic, as shown in Figure 4.1A. In addition, it was assumed that the
boundary conditions remain unchanged during the application of loading
on the finite element model. With these assumptions, the finite element
equilibrium equation was derived for static analysis as presented in Eq. (2.4).
The equation corresponds to linear analysis of a structural problem because
the displacement response {d} is a linear function of the applied force vector
{F}. This means that if the forces are increased with a constant factor, the
corresponding displacements will be increased with the same factor. On the
other hand, in nonlinear analysis, the aforementioned assumptions are not
valid. The assumption is that the displacement must be small so the evalua-
tion of the stiffness matrix [K] and the force vector {F} of Eq. (2.4) were
assumed to be constant and independent on the element displacements,
because all integrations have been performed over the original volume of
the finite elements and the strain�displacement relationships. The assump-
tion of a linear elastic material was implemented in the use of constant
stress�strain relationships. Finally, the assumption that the boundary condi-
tions remain unchanged was reflected in the use of constant restraint relations
for the equilibrium equation.
Recognizing the previous discussion, we can define three main non-
linear analyses commonly known as materially nonlinear analysis, geomet-
rically (large displacement and large rotation) nonlinear analysis, and
materially and geometrically nonlinear analysis. In materially nonlinear
56
Finite Element Analysis and Design of Metal Structures
DOI: http://dx.doi.org/10.1016/B978-0-12-416561-8.00004-4
© 2014 Elsevier Inc.
All rights reserved.
http://dx.doi.org/10.1016/B978-0-12-416561-8.00004-4
analysis, the nonlinear effect lies in the nonlinear stress�strain relation-
ship, with the displacements and strains being infinitesimally small, as
shown in Figure 4.1B. Therefore, the usual engineering stress and strain
measurements can be employed. In geometrically nonlinear analysis, the
structure undergoes large rigid body displacements and rotations, as
shown in Figure 4.1C. Majority of geometrically nonlinear analyses were
based on von Karman nonlinear equations such as the analyses presented
in Refs [4.1�4.8]. The equations allow coupling between bending and
membrane behavior with the retention of Kirchhoff normality constraint
[1.5]. Finally, materially and geometrically nonlinear analysis combines
both nonlinear stress�strain relationship and large displacements and
rotations experienced by the structure.
¤
 = F/A; = /E; = *L
A
F
; 
E
y for < y; 
t
yy
EE
 for y < 0.04 
 < 0.04 
E 
L 
F
Cross-sectional area = A 
1 2 
y 
x
Et
E 
y
y
y
x 
L 
1 
2 
F 
L 
F 
F 
x 
y
2 1 
(A)
(B)
(C)
Figure 4.1 Types of finite element analyses: (A) linear elastic analysis, (B) materially
nonlinear analysis, and (C) geometrically nonlinear analysis.
57Linear and Nonlinear Finite Element Analyses
This chapter starts by introducing linear eigenvalue buckling analysis,
which is required for modeling initial local and overall geometric imper-
fections as briefly mentioned in Section 3.5. After that, this chapter details
the nonlinear materialand geometry analyses required for simulating
actual performance of metal structures. Once again, this chapter explains
the analyses that are commonly incorporated in all efficient general-
purpose finite element software; however as an example, nonlinear analyses
used by ABAQUS [1.27] are particularly highlighted. Lastly, this chapter
presents the RIKS method used in ABAQUS [1.27] that can accurately
model the collapse behavior of metal structural members.
4.2. ANALYSIS PROCEDURES
Most available general-purpose finite element software divides the problem
history (overall finite element analysis) into different steps as shown in
Figure 4.2. An analysis procedure can be specified for each step, with pre-
scribing loads, boundary conditions, and output requests specified for each
step. A step is a phase of the problem history, and in its simplest form,
a step can be just a static analysis of a load changing from one magnitude to
another, as shown in Figure 4.2. For each step, one can choose an analysis
procedure. This choice defines the type of analysis to be performed during
the step such as static stress analysis, eigenvalue buckling analysis, or any
other types of analyses. It should be noted that as mentioned previously,
Displacement
Load
Ptotal
Step 1
P3
P2
P1
Problem
history
u1 u2 u3 utotal
Figure 4.2 Load�displacement history in a nonlinear analysis.
58 Finite Element Analysis and Design of Metal Structures
static stress analyses are only detailed in this book. Static analyses are used
when inertia effects can be neglected. The analyses can be linear or non-
linear and assume that time-dependent material effects, such as creep, are
negligible. Linear static analysis involves the specification of load cases and
appropriate boundary conditions. If all or part of a structure has linear
response, substructuring is a powerful capability for reducing the computa-
tional cost of large analyses. Static nonlinear analyses can also involve geo-
metrical nonlinearity and/or material nonlinearity effects. If geometrically
nonlinear behavior is expected in a step, the large-displacement formulation
should be used. Only one procedure is allowed per step and any combination
of available procedures can be used step by step. However, information from
a previous step can be imported to the current step by calling the results
from the previous step. The loads, boundary conditions, and output requests
can be inserted in any step.
Most available general-purpose finite element software classify the
steps into two main kinds of steps: general analysis steps and linear perturba-
tion steps. General analysis steps can be used to analyze linear or nonlinear
response. On the other hand, linear perturbation steps can be used only
to analyze linear problems. Linear analysis is always considered to be
linear perturbation analysis about the state at the time when the linear
analysis procedure is introduced. The linear perturbation approach allows
general application of linear analysis techniques in cases where the linear
response depends on preloading or on the nonlinear response history of
the model. In general analysis steps and linear perturbation steps, the solu-
tion to a single set of applied loads can be predicted. However, for static
analyses covered in this book, it is possible to find solutions to multiple
load cases. In this case, the overall analysis procedure can be changed
from step to step. This allows the state of the model (stresses, strains, dis-
placements, deformed shapes, etc.) to be updated throughout all general
analysis steps. The effects of previous history can be included in the
response in each new analysis step by calling the results of a previous his-
tory. As an example, after conducting an initial condition analysis step to
include residual stresses in cross sections, the initial stresses in the whole
cross section will be updated from zero to new applied stresses that
accounted for the residual stresses effect in metal structures.
It should be noted that linear perturbation steps have no effect on sub-
sequent general analysis steps and can be conducted separately as a whole
(overall) analysis procedure. In this case, the data obtained from the linear
perturbation steps can be saved in files that can be called into the
59Linear and Nonlinear Finite Element Analyses
subsequent general analysis steps. For example, linear eigenvalue buckling
analyses, needed for modeling of initial overall and local geometric
imperfections, can be conducted initially as a separate overall analysis pro-
cedure, and buckling modes can be extracted from the analyses and saved
in files. The saved files can be called into subsequent static general analy-
ses and factored to model initial geometric imperfections. The most obvi-
ous reason for using several steps in an analysis is to change the analysis
procedure type. However, several steps can also be used to change output
requests, such as the boundary conditions or loading (any information
specified as history, or step-dependent data). Sometimes, an analysis may
be progressed to a point where the present step definition needs to be
modified. ABAQUS [1.27] provides the ability to restart the analysis,
whereby a step can be terminated prematurely and a new step can be
defined for the problem continuation. History data prescribing the load-
ing, boundary conditions, and output will remain in effect for all subse-
quent general analysis steps until they are modified or reset. ABAQUS
[1.27] will compare all loads and boundary conditions specified in a step
with the loads and boundary conditions in effect during the previous step
to ensure consistency and continuity. This comparison is expensive if the
number of individually specified loads and boundary conditions is very
large. Hence, the number of individually specified loads and boundary
conditions should be minimized, which can usually be done by using
element and node sets instead of individual elements and nodes.
Most current general-purpose finite element software divides each step
of analysis into multiple increments. In most cases, one can choose either
automatic (direct) time incrementation or user-specified fixed time incrementation to
control the solution. Automatic time incrementation is a built-in incre-
mentation scheme that allows the software to judge the increment needed
based on equilibrium requirements. On the other hand, user-specified
fixed time incrementation forces the software to use a specified fixed
increment, which in many cases may be large, small, or need updating
during the step. This results in the analysis to be stopped and readjusted.
Therefore, automatic incrementation is recommended for most cases.
The methods for selecting automatic or direct incrementation are always
prescribed by all general-purpose software to help modelers. In nonlinear
analyses, most general-purpose software will use increment and iterate as
necessary to analyze a step, depending on the severity of the nonlinearity.
Iterations conducted within an increment can be classified as regular
equilibrium iterations and severe discontinuity iterations. In regular equilibrium
60 Finite Element Analysis and Design of Metal Structures
iterations, the solution varies smoothly, while in severe discontinuity itera-
tions abrupt changes in stiffness occur. The analysis will continue to iterate
until the severe discontinuities are sufficiently small (or no severe disconti-
nuities occur) and the equilibrium tolerances are satisfied. Modelers can
provide parameters to indicate a level of accuracy in the time integration,
and the software will choose the time increments to achieve this accuracy.
Direct user control is provided because it can sometimes save computa-
tional cost in cases where modelers are familiar with the problem and
know a suitable incrementation scheme. Modelers can define the upper
limitto the number of increments in an analysis. The analysis will stop if
this maximum is exceeded before the complete solution to the step has
been obtained. To reach a solution, it is often necessary to increase the
number of increments allowed by defining a new upper limit.
In nonlinear analyses, general-purpose software use extrapolation to
speed up the solution. Extrapolation refers to the method used to deter-
mine the first guess to the incremental solution. The guess is determined
by the size of the current time increment and by whether linear, parabolic,
or no extrapolation of the previously attained history of each solution
variable is chosen. Linear extrapolation is commonly used with 100%
extrapolation of the previous incremental solution being used at the start
of each increment to begin the nonlinear equation solution for the next
increment. No extrapolation is used in the first increment of a step.
Parabolic extrapolation uses two previous incremental solutions to obtain
the first guess to the current incremental solution. This type of extrapola-
tion is useful in situations when the local variation of the solution with
respect to the timescale of the problem is expected to be quadratic, such
as the large rotation of structures. If parabolic extrapolation is used in a
step, it begins after the second increment of the step, i.e., the first incre-
ment employs no extrapolation, and the second increment employs linear
extrapolation. Consequently, slower convergence rates may occur during
the first two increments of the succeeding steps in a multistep analysis.
Nonlinear problems are commonly solved using Newton’s method, and
linear problems are commonly solved using the stiffness method. Details
of the aforementioned solution methods are outside the scope of this
book; however, the methods are presented in detail in Refs [1.1�1.7].
Most general-purpose software adopt a convergence criterion for the solu-
tion to nonlinear problems automatically. Convergence criterion is the
method used by software to govern the balance equations during the iter-
ative solution. The iterative solution is commonly used to solve the
61Linear and Nonlinear Finite Element Analyses
equations of nonlinear problems for unknowns, which are the degrees of
freedom at the nodes of the finite element model. Most general-purpose
software have control parameters designed to provide reasonably optimal
solution to complex problems involving combinations of nonlinearities as
well as efficient solution to simpler nonlinear cases. However, the most
important consideration in the choice of the control parameters is that
any solution accepted as “converged” is a close approximation to the
exact solution to the nonlinear equations. Modelers can reset many
solution control parameters related to the tolerances used for equilibrium
equations. If less strict convergence criterion is used, results may be
accepted as converged when they are not sufficiently close to the exact
solution to the nonlinear equations. Caution should be considered when
resetting solution control parameters. Lack of convergence is often due to
modeling issues, which should be resolved before changing the accuracy
controls. The solution can be terminated if the balance equations failed to
converge. It should be noted that linear cases do not require more than
one equilibrium iteration per increment, which is easy to converge. Each
increment of a nonlinear solution will usually be solved by multiple
equilibrium iterations. The number of iterations may become excessive,
in which case the increment size should be reduced and the increment
will be attempted again. On the other hand, if successive increments are
solved with a minimum number of iterations, the increment size may be
increased. Modelers can specify a number of time incrementation control
parameters. Most general-purpose software may have trouble with the
element calculations because of excessive distortion in large-displacement
problems or because of very large plastic strain increments. If this occurs
and automatic time incrementation has been chosen, the increment will
be attempted again with smaller time increments.
4.3. LINEAR EIGENVALUE BUCKLING ANALYSIS
Eigenvalue buckling analysis is generally used to estimate the critical
buckling (bifurcation) load of structures. The analysis is a linear perturba-
tion procedure. The analysis can be the first step in a global analysis of an
unloaded structure or it can be performed after the structure has been
preloaded. It can be used to model measured initial overall and local geo-
metric imperfections or in the investigation of the imperfection sensitivity
of a structure in case of lack of measurements. Eigenvalue buckling is
generally used to estimate the critical buckling loads of stiff structures
62 Finite Element Analysis and Design of Metal Structures
(classical eigenvalue buckling). Stiff structures carry their design loads
primarily by axial or membrane action, rather than by bending action.
Their response usually involves very little deformation prior to buckling.
A simple example of a stiff structure is the stainless steel hollow section
columns presented in Figure 3.1, which responds very stiffly to a com-
pressive axial load until a critical load is reached, when it bends suddenly
and exhibits a much lower stiffness. However, even when the response of
a structure is nonlinear before collapse, a general eigenvalue buckling
analysis can provide useful estimates of collapse mode shapes.
The buckling loads are calculated relative to the original state of the
structure. If the eigenvalue buckling procedure is the first step in an
analysis, the buckled (deformed) state of the model at the end of the
eigenvalue buckling analysis step will be the updated original state of the
structure. The eigenvalue buckling can include preloads such as dead load
and other loads. The preloads are often zero in classical eigenvalue buck-
ling analyses. An incremental loading pattern is defined in the eigenvalue
buckling prediction step. The magnitude of this loading is not important;
it will be scaled by the load multipliers that are predicted by the eigen-
value buckling analysis. The buckling mode shapes (eigenvectors) are also
predicted by the eigenvalue buckling analysis. The critical buckling loads
are then equal to the preloads plus the scaled incremental load. Normally,
the lowest load multiplier and buckling mode are of interest. The
buckling mode shapes are normalized vectors and do not represent actual
magnitudes of deformation at critical load. They are normalized so that
the maximum displacement component has a magnitude of 1.0. If all
displacement components are zero, the maximum rotation component is
normalized to 1.0. These buckling mode shapes are often the most useful
outcome of the eigenvalue buckling analysis, since they predict the likely
failure modes of the structure.
Some structures have many buckling modes with closely spaced
eigenvalues, which can cause numerical problems. In these cases, it is
recommended to apply enough preload to load the structure to just
below the buckling load before performing the eigenvalue analysis. In
many cases, a series of closely spaced eigenvalues indicates that the
structure is imperfection sensitive. An eigenvalue buckling analysis will
not give accurate predictions of the buckling load for imperfection-
sensitive structures. In this case, the static Riks procedure, used by
ABAQUS [1.27], which will be highlighted in this chapter, should be
used instead. Negative eigenvalues may be predicted from an eigenvalue
63Linear and Nonlinear Finite Element Analyses
buckling analysis. The negative eigenvalues indicate that the structure
would buckle if the loads were applied in the opposite direction.
Negative eigenvalues may correspond to buckling modes that cannot be
understood readily in terms of physicalbehavior, particularly if a preload
is applied that causes significant geometric nonlinearity. In this case,
a geometrically nonlinear load�displacement analysis should be per-
formed. Because buckling analysis is usually done for stiff structures,
it is not usually necessary to include the effects of geometry change in
establishing equilibrium for the original state. However, if significant
geometry change is involved in the original state and this effect is con-
sidered to be important, it can be included by specifying that geometric
nonlinearity should be considered for the original state step. In such
cases, it is probably more realistic to perform a geometrically nonlinear
load�displacement analysis (Riks analysis) to determine the collapse
loads, especially for imperfection-sensitive structures as mentioned
previously. While large deformation can be included in the preload, the
eigenvalue buckling theory relies on there being little geometry change
due to the live (scaled incremental load) buckling load. If the live load
produces significant geometry changes, a nonlinear collapse (Riks) analysis
must be used.
The initial conditions such as residual stresses can be specified for an
eigenvalue buckling analysis. If the buckling step is the first step in the
analysis, these initial conditions form the original state of the structure.
Boundary conditions can be applied to any of the displacement or
rotation degrees of freedom (six degrees of freedom). Boundary condi-
tions are treated as constraints during the eigenvalue buckling analysis.
Therefore, the buckling mode shapes are affected by these boundary con-
ditions. The buckling mode shapes of symmetric structures subjected to
symmetric loadings are either symmetric or antisymmetric. In such cases,
it is more efficient to use symmetry to reduce the finite element mesh of
the model. Axisymmetric structures subjected to compressive loading
often collapse in nonaxisymmetric modes. Therefore, these structures
must be modeled as a whole. The loads prescribed in an eigenvalue buck-
ling analysis can be concentrated nodal forces applied to the displacement
degrees of freedom or can be distributed loads applied to finite element
faces. The load stiffness can be of a significant effect on the critical buck-
ling load. It is important that the structure is not preloaded above the
critical buckling load. During an eigenvalue buckling analysis, the model’s
response is defined by its linear elastic stiffness in the original state. All
64 Finite Element Analysis and Design of Metal Structures
nonlinear or inelastic material properties are ignored during an eigenvalue
buckling analysis. Any structural finite elements can be used in an eigenvalue
buckling analysis. The values of the eigenvalue load multiplier (buckling
loads) will be printed in the data files after the eigenvalue buckling analysis.
The buckling mode shapes can be visualized using the software. Any other
information such as values of stresses, strains, or displacements can be saved
in files at the end of the analysis.
Now, let us go back to the fixed-ended cold-formed stainless steel
rectangular hollow section column presented in Figure 3.1. It is possible
to explain how the eigenvalue buckling analysis has been used to model
initial overall and local geometric imperfections of stainless steel columns
presented by Ellobody and Young [1.30]. As mentioned previously, long
columns having compact cross sections with small overall depth to plate
thickness ratios (D/t) are likely to fail owing to overall flexural buckling.
On the other hand, long columns having slender or relatively slender
cross sections with large D/t ratios are likely to fail due to local buckling
or interaction of local and overall buckling. Both initial local and overall
geometric imperfections were found in the columns as a result of the
manufacturing, transporting, and fitting processes. Hence, superposition
of local buckling mode as well as overall buckling mode with measured
magnitudes is recommended [4.9,4.10] in the finite element modeling of
the column. These buckling modes can be obtained by carrying eigen-
value analyses of the column with large D/t ratio as well as small D/t ratio
to ensure local and overall buckling occurs, respectively. In this case, only
the lowest buckling mode (eigenmode 1) was used in the eigenvalue
buckling analyses. This technique is used in this study to model the initial
local and overall imperfections of the columns. Slender stub columns
having short lengths can be modeled for local imperfection only without
the consideration of overall imperfection. Since all buckling modes
predicted by ABAQUS [1.27] eigenvalue analysis are normalized to 1.0,
the buckling modes were factored by the measured magnitudes of the
initial local and overall geometric imperfections. Figure 4.3 shows the
local and overall imperfection buckling modes predicted for the column
presented in Figure 3.1.
4.4. MATERIALLY NONLINEAR ANALYSIS
Materially nonlinear analysis of metal structures is a general nonlinear
analysis step. The analysis can be also called load�displacement nonlinear
65Linear and Nonlinear Finite Element Analyses
material analysis and normally follows the linear eigenvalue buckling analy-
sis step or initial condition stress analysis. All required information regard-
ing the behavior of metal structures are predicted from the materially
nonlinear analysis. The information comprised the ultimate loads,
failure modes, and load�displacement relationships as well as any other
required data can be obtained from materially nonlinear analysis. The
initial overall and local geometric imperfections, residual stresses, and
nonlinear stress�strain curves of the construction material are included
in the load�displacement nonlinear material analysis. Since most, if not all,
metal structures have nonlinear stress�strain curves or linear�nonlinear
stress�strain curves, which are shown for examples in Figure 1.1, most
of the general nonlinear analysis steps associated with metal structures
are materially nonlinear analyses. Section 3.4 has previously detailed the
modeling of nonlinear material properties that should be included in the
materially nonlinear analyses.
(A) (B)
Figure 4.3 Buckling modes (eigenmode 1) for the column specimen presented in
Figure 3.1 and previously reported in Ref. [1.30]: (A) local imperfection and (B) overall
imperfection.
66 Finite Element Analysis and Design of Metal Structures
Materially nonlinear analysis (with or without consideration of geometric
nonlinearity) of metal structures is done to determine the overall response
of the structures. From a numerical viewpoint, the implementation of a non-
linear stress�strain curve of a construction metal material involves the integra-
tion of the state of the material at an integration point over a time increment
during a materially nonlinear analysis. The implementation of a nonlinear
stress�strain curve must provide an accurate material stiffness matrix for use in
forming the nonlinear equilibrium equations of the finite element formula-
tion. The mechanical constitutive models associated with metal structures in
ABAQUS [1.27] consider elastic and inelastic response of the material. The
inelastic response is commonly modeled with plasticity models as mentioned
previously in Chapter 3. In the inelastic response models that are provided in
ABAQUS [1.27], the elastic and inelastic responses are distinguished by sepa-
rating the deformation into recoverable (elastic) and nonrecoverable (inelastic)
parts. This separation is based on the assumption that there is an additive rela-
tionship between strain rates of the elastic and inelastic parts. The constitutive
material models used in most available general-purpose finite element software
are commonly accessed by any of the solid or structural elements previously
highlighted in Chapters2 and 3. This access is made independently at each
constitutive calculation point. These points are the numerical integration
points in the elements. The constitutive models obtain the state at the point
under consideration at the start of the increment from the material database
specified in the step. The state variables include the stresses and strains used in
the constitutive models. The constitutive models update the state of the mate-
rial response to the end of the increment. Some examples of materially non-
linear analyses are presented in Refs [4.11,4.12].
4.5. GEOMETRICALLY NONLINEAR ANALYSIS
Geometrically nonlinear analysis of metal structures is a general nonlinear
analysis step. The analysis can be also called load�displacement nonlinear
geometry analysis and normally follows the linear eigenvalue buckling anal-
ysis step or initial condition stress analysis. The initial overall and local
geometric imperfections and residual stresses are included in the
load�displacement nonlinear geometry analysis. If the stress�strain curve
of the construction metal material is nonlinear, the analysis will be called
combined materially and geometrically nonlinear analysis or load�displacement
nonlinear material and geometry analysis, as shown for examples in Refs
[4.13,4.14]. All required information regarding the behavior of metal
67Linear and Nonlinear Finite Element Analyses
structures are predicted from the combined materially and geometrically
nonlinear analysis. The information comprised the ultimate loads, failure
modes, and load�displacement relationships as well as any other required
data can be obtained from the combined materially and geometrically
nonlinear analysis.
In order to understand the geometrically nonlinear analysis, let us
imagine a simply supported beam subjected to lateral loads producing
only bending moments at small loads, as shown in Figure 4.4A. As deflec-
tions increase at higher loads, there will be membrane forces in addition
to bending moments. In this case, large displacements and rotations may
constitute a major part of the overall motion of the beam. If the lateral
deflection increases significantly, the classical theory of beams will be
inadequate and the second-order effect of the vertical displacements on
the membrane stresses needs to be considered. In addition, all classical
solutions for elastic beams will not be applicable to beams loaded beyond
the elastic limit. Further details in geometrically nonlinear analyses could
be found in Refs [1.1�1.7].
4.6. RIKS METHOD
The Riks method provided by ABAQUS [1.27] is an efficient method
that is generally used to predict unstable, geometrically nonlinear collapse
of a structure. The method can include nonlinear materials and boundary
conditions. The method commonly follows an eigenvalue buckling analy-
sis to provide complete information about a structure’s collapse. The Riks
method can be used to speed convergence of unstable collapse of struc-
tures. Geometrically nonlinear static metal structures sometimes involve
buckling or collapse behavior. Several approaches are possible for model-
ing such behavior. One of the approaches is to treat the buckling response
dynamically, thus actually modeling the response with inertia effects
L
L
(A) (B)
ω
Figure 4.4 Simply supported beam in a geometrically nonlinear analysis: (A) bending
moments expected only and (B) membrane forces and bending moments expected.
68 Finite Element Analysis and Design of Metal Structures
included as the structure snaps. This approach is easily accomplished by
restarting the terminated static procedure and switching to a dynamic
procedure when the static solution becomes unstable. In some simple
cases, displacement control can provide a solution, even when the conju-
gate load (the reaction force) is decreasing as the displacement increases.
Alternatively, static equilibrium states during the unstable phase of the
response can be found by using the modified Riks method supported by
ABAQUS [1.27]. This method is used for cases where the loading is pro-
portional, where the load magnitudes are governed by a single scalar
parameter. The method can provide solutions even in cases of complex,
unstable response such as that shown in Figure 4.5.
In simple structures, linear eigenvalue buckling analysis may be suffi-
cient for design evaluation. However, in complex structures involving
material nonlinearity, geometric nonlinearity prior to buckling, or
unstable postbuckling behavior, a load�displacement (Riks) analysis must
be performed to investigate the structures accurately. The Riks method
treats the load magnitude as an additional unknown and solves loads and
displacements simultaneously. Therefore, another quantity must be used
to measure the progress of the solution. ABAQUS [1.27] uses the arc
length along the static equilibrium path in load�displacement domain.
This approach provides solutions regardless of whether the response is
stable or unstable. If the Riks step is a continuation of a previous history,
any loads that exist at the beginning of the step are treated as dead loads
with constant magnitude. A load whose magnitude is defined in the Riks
Displacement
Load
P
A
Figure 4.5 Load�displacement behavior that could be predicted by the Riks method
(ABAQUS [1.27]).
69Linear and Nonlinear Finite Element Analyses
step is referred to as a reference load. All prescribed loads are ramped
from the initial (dead load) value to the reference values specified.
ABAQUS [1.27] uses Newton’s method to solve the nonlinear equilib-
rium equations. The Riks procedure uses very small extrapolation of the
strain increment. Modelers can provide an initial increment in arc length
along the static equilibrium path when defining the step. After that,
ABAQUS [1.27] computes subsequent steps automatically. Since the load-
ing magnitude is part of the solution, modelers need a method to specify
when the step is completed. It is common that one can specify a maxi-
mum displacement value at a specified degree of freedom. The step will
terminate once the maximum value is reached. Otherwise, the analysis
will continue until the maximum number of increments specified in the
step definition is reached.
The Riks method works well with structures having a smooth equilib-
rium path in load�displacement domain. The Riks method can be used to
solve postbuckling problems, both with stable and unstable postbuckling
behavior. In this way, the Riks method can be used to perform postbuck-
ling analyses of structures that show linear behavior prior to (bifurcation)
buckling. When performing a load�displacement analysis using the Riks
method, important nonlinear effects can be included. Imperfections based
on linear buckling modes can be also included in the analysis of structures
using the Riks method. It should be noted that the Riks method cannot
obtain a solution at a given load or displacement value since these are
treated as unknowns. Termination of the analysis using the Riks method
occurs at the first solution that satisfies the step termination criterion.
To obtain solutions at exact values of load or displacement, the analysis must
be restarted at the desired point in the step and a new, non-Riks step must
be defined. Since the subsequent step is a continuation of the Riks analysis,
the load magnitude in that step must be given appropriately so that the step
begins with the loading continuing to increase or decrease according to
its behavior at the point of restart. Initial values of stresses such as residual
stresses can be inserted in the analysis using the Riks method. Also, boundary
conditions can be applied to any of the displacement or rotation degrees
of freedom (six degrees of freedom). Concentrated nodal forces and
moments applied to associated displacement or rotation degrees of free-
dom (six degrees of freedom) as well as distributed loadsat finite element
faces can be inserted in the analysis using the Riks method. Nonlinear
material models that describe mechanical behavior of metal structures can
be incorporated in the analysis using the Riks method.
70 Finite Element Analysis and Design of Metal Structures
REFERENCES
[4.1] Murray, D. W. and Wilson, E. L. Finite element large deflection analysis of plates.
American Society of Civil Engineers, ASCE, 95(1), 143�165, 1969.
[4.2] Bergan, P. G. and Clough, R. W. Large deflection analysis of plates and shallow
shells using the finite element method. International Journal for Numerical
Methods in Engineering, 5, 543�556, 1973.
[4.3] Srinivasan, R. S. and Bobby, W. Nonlinear analysis of skew plates using the finite
element method. Composite Structures, 6, 199�202, 1976.
[4.4] Argyris, J. H., Dunne, P. C. and Scharpf, D. W. On large displacement-small strain
analysis of structures with rotational freedoms. Computer Methods in Applied
Mechanics and Engineering, 14, 401�451, 1978.
[4.5] Kondoh, K., Tanaka, K. and Atluri, S. N. An explicit expression for the tangent-
stiffness of a finitely deformed 3-D beam and its use in the analysis of space frames.
Composite Structures, 24, 253�271, 1986.
[4.6] Yang, Y. B. and McGuire, W. Joint rotation and geometric nonlinear analysis.
Journal of Structural Engineering, ASCE, 112, 879�905, 1986.
[4.7] Meek, J. L. and Loganathan, S. Geometrically non-linear behaviour of space frame
structures. Composite Structures, 31, 35�45, 1989.
[4.8] Surana, K. S. and Sorem, R. M. Geometrically non-linear formulation for three
dimensional curved beam elements with large rotations. International Journal for
Numerical Methods in Engineering, 28, 43�73, 1989.
[4.9] Ellobody, E. and Young, B. Behaviour of cold-formed steel plain angle columns.
Journal of Structural Engineering, ASCE, 131(3), 457�466, 2005.
[4.10] Young, B. and Ellobody, E. Buckling analysis of cold-formed steel lipped angle col-
umns. Journal of Structural Engineering, ASCE, 131(10), 1570�1579, 2005.
[4.11] Holzer, S. and Yoshbash, Z. The p-version of the finite element method in incre-
mental elasto-plastic analysis. International Journal for Numerical Methods in
Engineering, 39, 1859�1878, 1996.
[4.12] Duster, A. and Rank, E. The p-version of the finite element method compared to
an adaptive h-version for the deformation theory of plasticity. Computer Methods
in Applied Mechanics and Engineering, 190, 1925�1935, 2001.
[4.13] Kassimali, A. Large deformation analysis of elastic-plastic frames. Journal of
Structural Engineering, 109, 1869�1886, 1983.
[4.14] Nie, Q. and Niu, Q. p-Version large strain finite element formulation and applica-
tion in elastic-plastic deformation. Composite Structures, 65, 761�765, 1997.
71Linear and Nonlinear Finite Element Analyses
http://refhub.elsevier.com/B978-0-12-416561-8.00004-4/sbref1
http://refhub.elsevier.com/B978-0-12-416561-8.00004-4/sbref1
http://refhub.elsevier.com/B978-0-12-416561-8.00004-4/sbref1
http://refhub.elsevier.com/B978-0-12-416561-8.00004-4/sbref2
http://refhub.elsevier.com/B978-0-12-416561-8.00004-4/sbref2
http://refhub.elsevier.com/B978-0-12-416561-8.00004-4/sbref2
http://refhub.elsevier.com/B978-0-12-416561-8.00004-4/sbref2
http://refhub.elsevier.com/B978-0-12-416561-8.00004-4/sbref3
http://refhub.elsevier.com/B978-0-12-416561-8.00004-4/sbref3
http://refhub.elsevier.com/B978-0-12-416561-8.00004-4/sbref3
http://refhub.elsevier.com/B978-0-12-416561-8.00004-4/sbref4
http://refhub.elsevier.com/B978-0-12-416561-8.00004-4/sbref4
http://refhub.elsevier.com/B978-0-12-416561-8.00004-4/sbref4
http://refhub.elsevier.com/B978-0-12-416561-8.00004-4/sbref4
http://refhub.elsevier.com/B978-0-12-416561-8.00004-4/sbref5
http://refhub.elsevier.com/B978-0-12-416561-8.00004-4/sbref5
http://refhub.elsevier.com/B978-0-12-416561-8.00004-4/sbref5
http://refhub.elsevier.com/B978-0-12-416561-8.00004-4/sbref5
http://refhub.elsevier.com/B978-0-12-416561-8.00004-4/sbref6
http://refhub.elsevier.com/B978-0-12-416561-8.00004-4/sbref6
http://refhub.elsevier.com/B978-0-12-416561-8.00004-4/sbref6
http://refhub.elsevier.com/B978-0-12-416561-8.00004-4/sbref7
http://refhub.elsevier.com/B978-0-12-416561-8.00004-4/sbref7
http://refhub.elsevier.com/B978-0-12-416561-8.00004-4/sbref7
http://refhub.elsevier.com/B978-0-12-416561-8.00004-4/sbref8
http://refhub.elsevier.com/B978-0-12-416561-8.00004-4/sbref8
http://refhub.elsevier.com/B978-0-12-416561-8.00004-4/sbref8
http://refhub.elsevier.com/B978-0-12-416561-8.00004-4/sbref8
http://refhub.elsevier.com/B978-0-12-416561-8.00004-4/sbref9
http://refhub.elsevier.com/B978-0-12-416561-8.00004-4/sbref9
http://refhub.elsevier.com/B978-0-12-416561-8.00004-4/sbref9
http://refhub.elsevier.com/B978-0-12-416561-8.00004-4/sbref10
http://refhub.elsevier.com/B978-0-12-416561-8.00004-4/sbref10
http://refhub.elsevier.com/B978-0-12-416561-8.00004-4/sbref10
http://refhub.elsevier.com/B978-0-12-416561-8.00004-4/sbref11
http://refhub.elsevier.com/B978-0-12-416561-8.00004-4/sbref11
http://refhub.elsevier.com/B978-0-12-416561-8.00004-4/sbref11
http://refhub.elsevier.com/B978-0-12-416561-8.00004-4/sbref11
http://refhub.elsevier.com/B978-0-12-416561-8.00004-4/sbref12
http://refhub.elsevier.com/B978-0-12-416561-8.00004-4/sbref12
http://refhub.elsevier.com/B978-0-12-416561-8.00004-4/sbref12
http://refhub.elsevier.com/B978-0-12-416561-8.00004-4/sbref12
http://refhub.elsevier.com/B978-0-12-416561-8.00004-4/sbref13
http://refhub.elsevier.com/B978-0-12-416561-8.00004-4/sbref13
http://refhub.elsevier.com/B978-0-12-416561-8.00004-4/sbref13
http://refhub.elsevier.com/B978-0-12-416561-8.00004-4/sbref14
http://refhub.elsevier.com/B978-0-12-416561-8.00004-4/sbref14
http://refhub.elsevier.com/B978-0-12-416561-8.00004-4/sbref14
CHAPTER55
Examples of Finite Element
Models of Metal Columns
5.1. GENERAL REMARKS
The insight of the main analysis procedures associated with finite element
modeling of metal structures has been provided in earlier chapters; we
can now present some examples of different finite element models of
metal columns. The examples presented in this chapter have been pub-
lished in journal papers that successfully detailed the performance of metal
columns. It should be noted that the examples presented in this chapter
are arbitrarily chosen from the research conducted by the authors of this
book so that all related information regarding the finite element models
developed in the papers can be available to readers. The chosen finite
element models are columns constructed from different metals having dif-
ferent mechanical properties, different cross sections, different boundary
conditions, and different geometries. It should be also noted that when
presenting the previously published models, the main objective is not to
repeat the previous published information but to explain the fundamentals
of the finite element method used in developing the models.
This chapter first presents a survey of recently published numerical,
using finite element method, investigations on metal columns. After that,
the chapter presents four examples of finite element models previously
published by the authors for four different metal columns. The authors
will highlight in this chapter how the information presented in the previ-
ous chapters are used to develop the examples of finite element models
discussed here. The experimental investigations were simulated using the
developed finite element models based on the information provided in
this book. The finite element models were verified, and the results were
compared with design values calculated from current specifications are
presented in this chapter with clear references. The authors have an aim
that the presented examples highlighted in this chapter can explain to
readers the effectiveness of finite element models in providing detailed
data that augment experimental investigations conducted in the field.
72
Finite Element Analysis and Design of Metal Structures
DOI: http://dx.doi.org/10.1016/B978-0-12-416561-8.00005-6© 2014 Elsevier Inc.
All rights reserved.
http://dx.doi.org/10.1016/B978-0-12-416561-8.00005-6
The results are discussed to show the significance of the finite element
models in predicting the structural response of different metal structural
elements.
5.2. PREVIOUS WORK
Many finite element models were developed in the literature, with
detailed examples presented in the following paragraphs, to investigate the
behavior and design of metal columns. The aforementioned numerical
investigations were performed on metal columns of steel, cold-formed
steel, stainless steel, and aluminum alloy materials. Schmidt [5.1] has
presented a state-of-the-art review of available information regarding the
stability and design of steel shell structures. The review has focused on
the various approaches related to a numerical-based stability design. The
study [5.1] has credited the finite element analyses of stability problems of
metal structures detailed by Galambos [5.2]. The author has outlined that
the development of powerful computers and highly efficient numerical
techniques helped the calculation related to shell structures with compli-
cated geometry, dominant imperfection influences, and nonlinear load
carrying behavior. The study [5.1] has also highlighted that, in the last
decade, necessary numerical tools are in the hands of research academics
as well as in commercial finite element software such as ABAQUS [1.27]
and ANSYS [5.3] for ordinary structural design engineers. The study [5.1]
has also shown that the main task of the design engineer is to model
complicated metal structures or metal shells properly and to convert the
numerical output into the characteristic buckling strength of real shells,
which is needed for an equally safe and economic design as recom-
mended by Schmidt and Krysik [5.4]. Furthermore, the study [5.1] has
shown that numerical investigations have been incorporated in relevant
guidance in the draft of the European Code (EC3) BS EN 1993-1-6 [5.5]
for steel shell structures. The study [5.1] has discussed different numerical
approaches to shell buckling using commercial finite element general-
purpose software. The author has concluded the need for shell buckling
tests, with high quality to be used as physical verification benchmarks for
numerical models.
Narayanan and Mahendran [5.6] have detailed combined experimental
and numerical investigations highlighting the distortional buckling behav-
ior of different shapes of cold-formed steel columns. The authors have
carried out more than 15 tests on the columns having intermediate length
73Examples of Finite Element Models of Metal Columns
under axial compression for the verification of the finite element models.
The authors have determined the sections and buckling properties of the
columns using a finite strip analysis program called THIN-WALL devel-
oped by the University of Sydney. The numerical investigation performed
in the study [5.6] used the general-purpose software ABAQUS [1.27].
The developed finite element models have incorporated initial geometric
imperfections and residual stresses. The load�axial shortening and
load�strain relationships were predicted from the finite element models
and compared against test results. The authors have compared the ultimate
design load capacities predicted from the tests as well as finite element
analyses against the design strengths calculated using the Australian/New
Zealand Standard (AS/NZS) 4600 [5.7]. The study has used the developed
finite element models to perform parametric studies considering different
steel strengths, thicknesses, and column lengths. The 4-node 3D quadrilat-
eral shell elements with reduced integration (S4R5), refer to Section 3.2,
available in ABAQUS [1.27] library were used in the finite element analyses
performed in the study [5.6]. An eigenvalue buckling analysis, as detailed
in Section 4.3, was performed first to obtain the buckling loads and associ-
ated buckling modes. The authors have performed a series of convergence
studies, as shown in Section 3.3, to predict the reasonable finite element
mesh size, which was 53 5 mm. Elastic-perfectly plastic material properties
were assumed for all steel grades used in the tests and finite element analyses.
In the nonlinear analyses [5.6], initial local geometric imperfections were
modeled by providing initial out-of-plane deflections to the model. The first
elastic buckling mode shape was used to create the local geometric imperfec-
tions for the nonlinear analysis. The maximum amplitude of the buckled
shape determined the degree of imperfection. The maximum value of dis-
tortional imperfection was taken based on the recommendations by Schafer
and Peköz [5.7] and Kwon and Hancock [5.8]. The study [5.6] did not
include any overall geometric imperfections in the finite element analyses.
The residual stresses were modeled using the INITIAL CONDITIONS
option with TYPE5 STRESS, USER available in ABAQUS [1.27], as
detailed in Section 3.6. The user-defined initial stresses were created using
the SIGINI Fortran user subroutine.
Raftoyiannis and Ermopoulos [5.9] have studied the elastic stability of
eccentrically loaded steel columns with tapered and stepped cross sections.
The initial geometric imperfection was incorporated in the analysis
assuming a parabolic shape according to EC3 [5.10]. A nonlinear finite
element analysis was employed by the authors to predict the plastic loads
74 Finite Element Analysis and Design of Metal Structures
and buckling behavior of the columns. The nonlinear analyses were
performed using a finite element package [5.11]. The flanges and web of
the steel columns were modeled with flat quadrilateral 3D shell elements.
An incremental procedure was employed for the applied load until a failure
mode was reached. The geometrical nonlinearity with large displacements
was considered in the finite element analyses using the updated Lagrange
method for solution to the nonlinear problem [1.1�1.7].
Zhu and Young [5.12] have presented a numerical investigation on
fixed-ended aluminum alloy tubular columns of square and rectangular
hollow sections. The columns investigated [5.12] were fixed-ended col-
umns with both ends transversely welded to aluminum end plates. The
failure modes predicted from the finite element analyses comprised local
buckling, flexural buckling, and interaction of local and flexural buckling.
The initial local and overall geometric imperfections were incorporated
in the finite element analyses as detailed in Ref. [5.12]. The material
nonlinearity of aluminum alloy was considered in the analysis. The load-
shortening curves predicted by the finite element analysis were compared
against test results. The 4-node doubly curved shell elements with
reduced integration (S4R) were used in the model based on the previous
recommendations given by Yan and Young [5.13] and Ellobody and
Young [1.30]. The size of the finite element mesh used in [5.12] was
103 10 mm (length by width), which was used in the modeling of the
columns. The same size has been previously used to simulate axially
loaded fixed-ended columns and shown to provide good simulation
results [5.13]. Both initial local and overall geometric imperfections were
incorporated in the model. Superposition of local buckling mode and
overall buckling mode with the measured magnitudes was carried out,
as discussed in Section 3.5. The buckling modes were obtained by
eigenvalue buckling analysis of the columns with very high value of
width-to-thickness ratio and very low value of width-to-thickness ratio
to ensure local and overall buckling occurs, respectively. Only the lowest
buckling mode (eigenmode 1) was used in the eigenvalue analysis.
Residual stresses were not included in the finite element model [5.12]
because in extruded aluminum alloy profiles, residual stresses are small
and can be neglected as recommended in Ref.[5.14].
The structural performance of cold-formed stainless steel slender and
nonslender circular hollow section columns was previously investigated by
Young and Ellobody [5.15] and Ellobody and Young [5.16], respectively,
through numerical investigations. Nonlinear 3D finite element models were
75Examples of Finite Element Models of Metal Columns
developed by the authors highlighting the behavior of the normal strength
austenitic stainless steel type 304 and the high strength duplex (austenitic-
ferritic approximately equivalent to EN 1.4462 and UNS S31803) columns.
The columns were compressed between fixed ends at different column
lengths. The geometric and material nonlinearities have been included in
the finite element analysis. The column strengths and failure modes were
predicted. An extensive parametric study was carried out to study the effects
of normal and high strength materials on cold-formed stainless steel non-
slender circular hollow section columns. The column strengths predicted
from the finite element analysis were compared with the design strengths
calculated using the American Specification [5.17], Australian/New
Zealand Standard [5.18], and European Code [5.19] for cold-formed
stainless steel structures. The numerical investigations [5.15, 5.16] have
proposed improved design equations for cold-formed stainless steel slender
and nonslender circular hollow section columns, respectively. The finite
element analyses performed in Refs [15.15, 15.16] have used ABAQUS
[1.27]. The finite element models were verified against the tests conducted
by Young and Hartono [5.20] on cold-formed stainless steel circular
hollow section columns.
The developed finite element models used the measured geometry,
initial local, and overall geometric imperfections and material properties.
The 4-node doubly curved shell elements with reduced integration (S4R)
was used to model the buckling behavior of fixed-ended cold-formed
stainless steel circular hollow section columns. The mesh size used in the
model was approximately 103 10 mm (length by width). The load was
applied in increments using the modified Riks method, as detailed in
Section, available in the ABAQUS [1.27] library. The nonlinear geometry
parameter (�NLGEOM) was included to deal with the large displacement
analysis. The load application and boundary conditions were identical to
the tests [5.20]. The measured stress�strain curves of circular stainless
steel tubes [5.20] were used in the analysis. Both initial local and overall
geometric imperfections were found in the column specimens. Hence,
superposition of local buckling mode as well as overall buckling mode
with measured magnitudes was used in the finite element analysis. These
buckling modes were obtained by carrying eigenvalue analyses of the
column with large external diameter to plate thickness ratio (D/t) as well
as small D/t ratio to ensure local and overall buckling occurs, respectively.
Only the lowest buckling mode (eigenmode 1) was obtained from the
eigenvalue analyses. Previous studies by Gardner [5.21], and Ellobody and
76 Finite Element Analysis and Design of Metal Structures
Young [1.30] on cold-formed stainless steel square and rectangular hollow
section columns have shown that the effect of residual stresses on the
column ultimate load is considered to be quite small. The cold-formed
square hollow section is formed by cold-rolling with welds of annealed
flat strip into a circular hollow section, and then further rolled into square
hollow section. Hence, the effect of residual stresses on the strength and
behavior of cold-formed stainless steel circular hollow section columns
would be even smaller than the square and rectangular hollow section
columns. Therefore, in order to avoid the complexity of the analysis, the
residual stresses were not included in the finite element analysis of cold-
formed stainless steel circular hollow section columns performed in Refs
[5.15, 5.16].
The buckling analysis of cold-formed high strength stainless steel
stiffened and unstiffened slender hollow section columns was highlighted
by Ellobody [5.22] through numerical investigation. Nonlinear 3D finite
element models were developed by the author to highlight the structural
benefits of using stiffeners to strengthen slender square and rectangular
hollow section columns. The construction material was high strength
duplex stainless steel, which is austenitic-ferritic stainless steel that is
approximately equivalent to EN 1.4462 and UNS S31803. The columns
were compressed between fixed ends at different column lengths. The
column strengths, load-shortening curves as well as failure modes were
predicted for the stiffened and unstiffened slender hollow section col-
umns. An extensive parametric study was conducted to study the effects
of cross section geometries on the strength and behavior of the stiffened
and unstiffened columns. The investigation has shown that the high
strength stainless steel stiffened slender hollow section columns offer a
considerable increase in the column strength over that of the unstiffened
slender hollow section columns. The column strengths predicted from
the parametric study were compared with the design strengths calculated
using the American Specification [5.17], Australian/New Zealand
Standard [5.18], and European Code [5.19] for cold-formed stainless steel
structures. The study [5.22] has shown that the design strengths obtained
using the three specifications are generally conservative for the cold-
formed stainless steel unstiffened slender square and rectangular hollow
section columns, but slightly unconservative for the stiffened slender
square and rectangular hollow section columns. The 4-node doubly
curved shell elements with reduced integration (S4R) were used to model
the buckling behavior of the stiffened columns. The mesh size used in the
77Examples of Finite Element Models of Metal Columns
model was approximately 203 10 mm (length by width). The load was
applied in increments using the modified Riks method available in the
ABAQUS [1.27] library. The nonlinear geometry parameter (�NLGEOM)
was included to deal with the large displacement analysis. Both initial
local and overall geometric imperfections were found in the column
specimens.
Zhang et al. [5.23] have presented combined experimental and
numerical investigations on cold-formed steel channels with inclined sim-
ple edge stiffeners compressed between pinned ends. The experimental
investigation comprised a total of 36 channel specimens having different
cross sections with different edge stiffeners. The initial geometric imper-
fections and material properties of the specimens were measured in
[5.23]. The failure modes predicted included local buckling, distortional
buckling, flexural buckling, and interaction of these buckling modes. The
study has indicated that inclined angle and loading position significantly
affect the ultimate load-carrying capacity and failure mode of the
channels. The numerical investigation presented in Ref. [5.23] proposed
a nonlinear finite element model, which was verified against the tests.
Geometric and material nonlinearities were included in the model. The
4-node 3D quadrilateral shell element with six degrees of freedom at
each node (S4), as detailed in Section 3.2, was used in the finite element
analyses. Eigenvalue buckling analyses and nonlinear load�displacement
analyses were conducted in the study [5.23]. By varying the size of the
elements, the finite element mesh used in the model was studied. It was
found that good simulation results could be obtained by using the ele-
ment size of approximately 203 10 mm (length by width) for the lip and
203 16 mm for the flange and web.
Becque and Rasmussen [5.24] have detailed a finite element model
studying the interaction of local and overall buckling in stainless steel
columns. The model incorporatednonlinear stress�strain behavior,
anisotropy, enhanced corner properties, and initial imperfections. The
model was verified against tests on stainless steel lipped channels. The
finite element model was further used in parametric studies, varying both
the cross-sectional slenderness and the overall slenderness. Three stainless
steel alloys were considered in the finite element analyses. The results
were compared with the governing design rules of the Australian [5.18],
North American [5.17], and European [5.19] standards for stainless steel
structures. A 4-node shell element with reduced integration (S4R) was
selected from the ABAQUS [1.27] element library to model the columns.
78 Finite Element Analysis and Design of Metal Structures
Gao et al. [5.25] have studied the load-carrying capacity of thin-walled
box-section stub columns fabricated by high strength steel through experi-
mental and numerical investigations. The columns investigated were axially
loaded having different geometries. The column strengths obtained from
the study [5.25] were compared with the design strengths predicted using
the American Iron and Steel Institute (AISI) code [5.26]. The finite element
analyses have used a general-purpose software ANSYS [5.3]. Parametric
studies were performed to investigate the ultimate strength of the high
strength steel stub columns. The authors have proposed a formula to predict
the loading capacity of the high strength steel stub column based on the
experimental and numerical investigations. Both material and geometric
nonlinearities were adopted in the calculations. Initial local and overall
geometric imperfections were included in the finite element model. The
residual stresses were also incorporated in the finite element model.
Theofanous and Gardner [5.27] have detailed combined experimental
and numerical investigations highlighting the compressive structural
response of the lean duplex stainless steel columns. The authors have
carried out a total of 8 stub column tests and 12 long column tests on
lean duplex stainless steel square and rectangular hollow sections. The
mechanical material properties, geometric properties, and assessment of
local and global geometric imperfections were measured in the study
[5.27]. Nonlinear finite element analyses and parametric studies were
performed to generate results over a wide range of cross-sectional and
member slenderness. The authors have used the experimental and numer-
ical results to assess the applicability of the Eurocode 3: Part 1�4 [5.19]
provisions regarding the Class 3 slenderness limit and effective width for-
mula for internal elements in compression and the column buckling curve
for hollow sections to lean duplex structural components. The authors
have used the published test data to validate the finite element models.
The general-purpose finite element software ABAQUS [1.27] was used
for all numerical studies reported in the paper. The finite element simula-
tions followed the proposals regarding numerical modeling of stainless
steel components previously reported by one of the authors in Refs
[5.28,5.29]. The measured geometric properties for stub columns and
long columns have been employed in the finite element models. The
4-node doubly curved shell element with reduced integration S4R has
been used in the study [5.27]. The authors have noted that the geometry,
boundary conditions, applied loads, and failure modes of the tested com-
ponents were symmetric; therefore, symmetry was exploited in the finite
79Examples of Finite Element Models of Metal Columns
element modeling with suitable boundary conditions applied along the
symmetry axes, enabling significant savings in computational time. In the
stub columns [5.27], only a quarter of the section was modeled, whereas
for the long columns, half of the cross section was discretized. For both
stub columns and long columns, the full length of component was mod-
eled. All degrees of freedom were restrained at the end cross sections of
the stub column models, apart from the vertical translation at the loaded
end, which was constrained via kinematic coupling to follow the same
vertical displacement.
Goncalves and Camotim [5.30] have presented a geometrically and
materially nonlinear generalized beam theory formulation. The finite ele-
ment analysis presented aimed to evaluate nonlinear elastoplastic equilib-
rium paths of thin-walled metal bars and associated collapse loads. This
finite element investigation was an extension to previously reported study
by the authors [5.31] by including the geometrically nonlinear effects.
The authors have assumed that the plate-like bending strains are assumed
to be small, but the membrane strains are calculated exactly. The study
used both stress-based and stress resultant-based generalized beam theory
approaches in a 3-node beam finite element. The study has shown that
the stress-based formulation is generally more accurate, but the stress
resultant-based formulation makes it possible to avoid numeric integration
in the through-thickness direction of the walls. The investigation [5.30]
comprised several numerical examples. The results obtained from the
study were also compared with that obtained using standard 2D solid and
shell finite element analyses.
5.3. FINITE ELEMENT MODELING AND EXAMPLE 1
The first example presented in this chapter is for cold-formed high
strength stainless steel columns, which were occasionally mentioned in
the previous chapters for explanation. The column tests were carried out
by Young and Lui [1.28,1.29] and provided the experimental ultimate
loads and failure modes of columns compressed between fixed ends, as
shown in Figure 3.1. The stainless steel columns had square and rectangu-
lar hollow sections having different geometries and lengths. The details of
column specimens were found in [1.28,1.29] and no intention to repeat
the published information in this book. However, it should be mentioned
that the experimental program presented was well planned such that
22 tests were carefully conducted. The tests were also well instrumented
80 Finite Element Analysis and Design of Metal Structures
such that the experimental results were used in the verification of the
finite element models developed by Ellobody and Young [1.30]. The
experimental program presented in [1.28,1.29] agrees well with the crite-
ria previously discussed, in Section 1.3, for a successful experimental
investigation. The cross section dimensions, material properties of the flat
and corner portions of the specimens, initial local and overall geometric
imperfections as well as residual stresses were measured as detailed in
[1.28,1.29]. The results obtained from the tests [1.28,1.29] included the
column strengths, load�axial shortening relationships and failure modes,
which once again conforms to the criteria mentioned in Section 1.3. The
results obtained have provided enough information for finite element
models to be developed.
The tests reported by Young and Lui [1.28,1.29] were modeled by
Ellobody and Young [1.30]. The general-purpose finite element software
ABAQUS [1.27] was used to simulate the cold-formed high strength stain-
less steel columns. The authors have developed a nonlinear finite element
model that accounted for the measured geometry, initial local and overall
geometric imperfections, residual stresses, and nonlinear material proper-
ties. The authors have performed two types of analyses. The first analysis
was eigenvalue buckling analysis, which is mentioned previously as linear
elastic analysis performed using the (�BUCKLE) procedure available in the
ABAQUS [1.27] library. The second analysis was the load�displacement
geometrically and materially nonlinear analysis, which follows the eigen-
value buckling analysis. The ultimate loads, failure modes, and axial short-
enings as well as any other required data were determinedfrom the second
analysis. The initial imperfections, residual stresses, and material nonlinearity
were also included in the second analysis.
The 4-node doubly curved shell elements with reduced integration
(S4R) were used in Ref. [1.30] to model the buckling behavior of cold-
formed high strength stainless steel columns. In order to choose the finite
element mesh that provides accurate results with minimum computational
time, convergence studies were conducted by the authors. It was found
that the mesh size of 203 10 mm (length by width) provides adequate
accuracy and minimum computational time in modeling the flat portions
of cold-formed high strength stainless steel columns, while finer mesh
was used at the corners. The boundary conditions and load application
were identical to the tests [1.28,1.29]. The load was applied in increments
using the modified Riks method available in the ABAQUS [1.27] library.
The nonlinear geometry parameter (�NLGEOM) was included to deal
81Examples of Finite Element Models of Metal Columns
with the large displacement analysis. The measured stress�strain curves for
flat and corner portions of the specimens [1.28,1.29] were used in the finite
element analyses [1.30]. The material behavior provided by ABAQUS
[1.27] allows for a multilinear stress�strain curve to be used, as described in
Section 3.4. Cold-formed high strength stainless steel columns with large
overall depth-to-plate thickness (D/t) ratio are likely to fail by local buckling
or interaction of local and overall buckling depending on the column
length and dimension. On the other hand, columns with small D/t ratio
are likely to fail by yielding or overall buckling. Both initial local and
overall geometric imperfections were found in the tested columns. Hence,
superposition of local buckling mode as well as overall buckling mode
with measured magnitudes was used in the finite element analyses. These
buckling modes were obtained from the eigenvalue buckling analyses of
the column with large D/t ratio as well as small D/t ratio to ensure local
and overall buckling occurs, respectively. Only the lowest buckling mode
(eigenmode 1) was used in the eigenvalue analyses.
The measured residual stresses [1.28,1.29] were included in the finite
element model to ensure accurate modeling of the behavior of cold-
formed high strength stainless steel columns. Measured residual stresses
were implemented in the finite element model by using the ABAQUS
(�INITIAL CONDITIONS, TYPE5 STRESS) parameter (see details in
Section). The material tests of flat and corner coupons considered the
effect of bending residual stresses; hence, only the membrane residual
stresses were modeled in this study. The magnitudes and distributions
of the membrane residual stresses in the flat and corner portions of the
columns were reported by Young and Lui [1.28,1.29]. A preliminary load
step to allow equilibrium of the residual stresses was defined before the
application of loading.
In the verification of the finite element model [1.30], a total of 22
cold-formed high strength stainless steel columns were analyzed. A com-
parison between the experimental and finite element analysis results was
carried out. The main objective of this comparison is to verify and check
the accuracy of the finite element model. The comparison of the ultimate
test and finite element analysis loads (PTest and PFE), load�axial shorten-
ing relationships from the tests, and finite element analysis and failure
modes obtained experimentally and numerically were compared in Ref.
[1.30]. The comparison of the ultimate loads has shown that good agree-
ment has been achieved between both results for most of the columns.
A maximum difference of 8% was observed between experimental and
82 Finite Element Analysis and Design of Metal Structures
numerical results. Three failure modes observed experimentally were
verified by the finite element model. The failure modes were yielding
failure (Y), local buckling (L), and flexural buckling (F). Figure 5.1 shows
the deformed shape of rectangular hollow section column having a length
of 3000 mm and the cross section dimensions shown in Figure 3.1,
observed experimentally and numerically using the finite element model.
The failure modes observed in the test and confirmed using the finite
element analysis were interaction of local and flexural buckling (L1 F).
It can be seen that the finite element model accurately predicted the
failure modes of the column observed in the test.
The study [1.30] has also investigated the effect of residual stresses on
the behavior of cold-formed high strength stainless steel columns of
duplex material. It has shown that the measured membrane residual
Figure 5.1 Comparison of experimental analysis (A) and finite element analysis (B) failure
modes of high strength rectangular hollow section stainless steel column [1.30].
83Examples of Finite Element Models of Metal Columns
stresses have a negligible effect on the ultimate load and load-shortening
behavior. In Figure 5.2, the load versus axial shortening of the column
having the cross section dimensions shown in Figure 3.1, and a length of
600 mm is presented. The curves were plotted with and without the sim-
ulation of the membrane residual stresses. It has shown that the ultimate
load and behavior of the columns are almost identical. Therefore, in order
to avoid the complexity of the analysis, the authors did not include the
residual stresses in the parametric studies.
Following the verification of the finite element model, the authors
[1.30] have performed parametric studies to study the effects of cross sec-
tion geometries on the strength and behavior of the columns. A total of
42 columns were analyzed in the parametric study to generate more data
outside the range covered by the experimental investigation [1.28,1.29].
The ultimate loads (PFE) and failure modes were predicted from the
parametric studies, which were considered as new information regarding
the high strength stainless steel columns investigated. The results obtained
from the parametric study can be used to extend the limits of design spec-
ified in the current codes of practice as conducted in the study [1.30].
The column strengths predicted from the parametric studies were com-
pared with the unfactored design strengths calculated using the American
[5.17], Australian/New Zealand [5.18], and European [5.19] specifications
for cold-formed stainless steel structures. Table 5.1 shows an example
of the comparison between the column strengths obtained from finite
element analysis (PFE) and design calculations, the nominal (unfactored)
design strengths PASCE obtained using the American Specification [5.17],
0
100
200
300
400
500
600
0 2 4 6 8
Shortening (mm)
Lo
ad
 (
kN
)
No residual stresses
Residual stresses
Figure 5.2 Load�axial shortening curves of high strength rectangular hollow section
stainless steel column having a length of 600 mm [1.30].
84 Finite Element Analysis and Design of Metal Structures
PAS/NZS obtained using the Australian/New Zealand Standard [5.18], and
PEC3 obtained using the European Code [5.19]. The example shown in
Table 5.1 is a rectangular hollow section column, as shown in Figure 3.1,
having an overall depth (D) of 90 mm, overall width (B) of 45 mm, and a
plate thickness of 3 mm. The column strengths were also plotted on the
vertical axis of Figure 5.3, as reported in Ref. [1.30], while the horizontal
axis was plotted as the effective length (le) that is assumed equal to
one-half of the column length for the fixed-ended columns.
Table 5.1 Comparison of Column Strengths Obtained from Finite Element Analysis
and Design Specifications for High Strength Rectangular Hollow Section Stainless
Steel Columns [1.30]
Specimen PFE (kN) PASCE (kN) PAS/NZS (kN) PEC3 (kN)
PFE
PASCE
PFE
PAS=NZS
PFE
PEC3
RT3L300 392.5 398.5 398.5 398.5 0.98 0.98 0.98
RT3L650376.3 398.5 398.5 398.5 0.94 0.94 0.94
RT3L1000 355.8 397.4 398.5 390.2 0.90 0.89 0.91
RT3L1500 327.6 330.0 318.1 333.9 0.99 1.03 0.98
RT3L2000 299.7 278.4 264.0 268.0 1.08 1.14 1.12
RT3L2500 274.6 234.5 214.4 207.0 1.17 1.28 1.33
RT3L3000 217.3 193.8 170.7 158.4 1.12 1.27 1.37
Mean � � � � 1.03 1.08 1.09
COV � � � � 0.097 0.145 0.172
0
100
200
300
400
500
600
0 500 1000 1500 2000
Effective length, le (mm)
A
xi
al
 lo
ad
, P
 (
kN
)
PFE
Flexural buckling 
PAS/NZS
PASCE
PEC3
Figure 5.3 Comparison of column strengths obtained from finite element analysis
and design specifications for high strength stainless steel columns [1.30].
85Examples of Finite Element Models of Metal Columns
5.4. FINITE ELEMENT MODELING AND EXAMPLE 2
The second example presented in this chapter is the aluminum alloy
columns, which was carried out by Zhu and Young [5.32] and provided
the experimental ultimate loads, load�axial shortening relationships and
failure modes of the aluminum alloy columns. The authors have used the
test results to develop a nonlinear finite element model simulating the
buckling behavior of the columns as detailed in [5.12]. The tested
columns [5.32] had square and rectangular hollow sections and were
compressed between fixed ends, as shown in Figure 5.4. The test speci-
mens were fabricated by extrusion using normal strength 6063-T5 and
high strength 6061-T6 heat-treated aluminum alloys. The test program
included 25 fixed-ended columns with both ends welded to aluminum
end plates, and 11 fixed-ended columns without the welding of end plates.
Therefore, the authors have used in Ref. [5.12] the term “welded column,”
which refers to a specimen with transverse welds at the ends of the column,
whereas the term “nonwelded column” refers to a specimen without trans-
verse welds. The testing condition of the welded and nonwelded columns is
identical, other than the absence of welding in the nonwelded columns. The
details of column specimens were found in Ref. [5.32] and, once again,
no intention to repeat the published information in this book. Details should
Aluminum alloy tube 
(B)
D 
B 
S S 
(A)
L 
Given: 
D=100 mm, B=44 mm,
and t=1.2 mm
t 
(C)
Aluminum alloy tube
D 
t 
D 
Figure 5.4 Example 2 of a fixed-ended aluminum alloy rectangular hollow section
column [5.12,5.32]. (A) Fixed-ended rectangular hollow section column. (B) Rectangular
hollow section (section S-S). (C) Square hollow section (section S-S).
86 Finite Element Analysis and Design of Metal Structures
be referred to Refs [5.12,5.32]. However, it should be mentioned that the
experimental program presented was well planned such that 25 tests were
accurately conducted. The tests were well instrumented such that the experi-
mental results were used in the verification of the finite element models
developed by Zhu and Young [5.12]. The nonwelded and welded material
properties for each series of specimens were determined by longitudinal
tensile coupon tests as detailed by Zhu and Young [5.32]. Initial overall
geometric imperfections were measured for all specimens prior to testing.
Initial local geometric imperfections were also measured for some specimens.
The details of the measurements were found by Zhu and Young [5.32].
The general-purpose finite element software ABAQUS [1.27] was used
in the analysis for the simulation of aluminum alloy fixed-ended columns
tested by Zhu and Young [5.32]. The measured geometry, initial overall and
local geometric imperfections, and material properties of the test specimens
were used in the finite element model. The model was based on the center-
line dimensions of the cross sections. Residual stresses were not included in
the model. This is because in extruded aluminum alloy profiles, whatever
be the heat treatment, residual stresses have very small values; for practical
purpose, these have a negligible effect on load-bearing capacity [5.14]. The
authors have also performed two types of analyses. The first analysis was
eigenvalue buckling analysis (see Section 4.3) which is as previously men-
tioned a linear elastic analysis performed using the (�BUCKLE) procedure
available in the ABAQUS [1.27] library. The second analysis was the
load�displacement geometrically and materially nonlinear analysis, which
follows the eigenvalue buckling analysis. The ultimate loads, failure modes,
and axial shortenings as well as any other required data were determined
from the second analysis. The initial imperfections and material nonlinearity
were also included in the second analysis.
The 4-node doubly curved shell elements with reduced integration
(S4R) were used in Ref. [5.12] to model the buckling behavior of the
aluminum alloy columns. The size of the finite element mesh of 103 10 mm
(length by width) was used in the modeling of the columns. The authors
have mentioned that the heat-treated aluminum alloys suffer loss of strength
in a localized region when welding is involved, and this is known as
heat-affected zone (HAZ) softening. The welded columns were modeled
by dividing the columns into different portions along the column length so
that the HAZ softening at both ends of the welded columns was included
in the simulation. The welded columns were separated into three parts,
the HAZ regions at both ends of the columns, and the main body of
87Examples of Finite Element Models of Metal Columns
the columns that are not affected by welding. Different mesh sizes were
considered in the HAZ regions. The authors have noted that the American
Specification [5.33] and Austrian/New Zealand Standard [5.34] for alumi-
num structures specified that the HAZ shall be taken as 1 in. (25.4 mm).
However, the European Code [5.35] for aluminum structures assumed the
HAZ extends to 30 mm for a TIG weld while the section thickness is less
than 6 mm.
The boundary conditions and load application were identical to the
tests [5.32]. The load was applied in increments using the modified Riks
method, available in the ABAQUS [1.27] library. The nonlinear geome-
try parameter (�NLGEOM) was included to deal with the large dis-
placement analysis. The measured stress�strain curves of the aluminum
alloy specimens [5.32] were used in the finite element analyses [5.12].
The material behavior provided by ABAQUS [1.27] allows for a multi-
linear stress�strain curve to be used.
The developed nonlinear finite element model detailed in Ref. [5.12]
was verified against the experimental results [5.32]. The authors have
compared the ultimate loads obtained numerically (PFEA) with that
obtained experimentally (PExp), and good agreement was achieved. The
mean value of PExp/PFEA ratio was 1.02 with the corresponding coeffi-
cient of variation (COV) of 0.045 for the nonwelded columns, as
discussed in [5.12]. For the welded columns, both the ultimate loads
predicted by the finite element analysis using the HAZ extension of
25 mm (PFEA25) and 30 mm (PFEA30) were compared with the experi-
mental results. The authors have shown that the PFEA25 are in better
agreement with the experimental ultimate loads compared with the
PFEA30. The observed failure modes obtained experimentally [5.32] and
confirmed numerically [5.12] included local buckling (L), flexural buck-
ling (F), interaction of local and flexural buckling (L1 F), and failure in
the HAZ. Figure 5.5 shows the comparison of the failure modes obtained
from the test and predicted by the finite element analysis, as previously
published in [5.12], for the high strength aluminum alloy nonwelded
rectangular hollow section specimen having an overall depth (D) of 100,
overall width (B) of 44, plate thickness (t) of 1.2, and a length of
1000 mm. Figure 5.6 shows the load-shortening curves obtained experi-
mentally and numerically for the high strength aluminum alloy welded
rectangular hollow section specimen having a D of 100, B of 44, t of 1.2,
and a length of 2350 mm. The load-shorteningcurves predicted by the
finite element analysis using the HAZ extension of 25 and 30 mm are
88 Finite Element Analysis and Design of Metal Structures
Figure 5.5 Comparison of failure modes obtained from experimental analysis (A) and
finite element analysis (B) of rectangular hollow section aluminum alloy column having
a length of 1000 mm [5.12].
35
30
25
20
15
10
5
0
0 1 2 3 4 5
A
xi
al
 lo
ad
, P
 (
kN
)
Axial shortening, e (mm)
FEA25
FEA30
Test
Figure 5.6 Load�axial shortening curves obtained experimentally and numerically for
rectangular hollow section aluminum alloy column having a length of 2350 mm [5.12].
89Examples of Finite Element Models of Metal Columns
shown in Figure 5.6. The authors have shown that good agreement was
found between the experimental and numerical curves, which demon-
strated the reliability of the finite element analysis predictions.
5.5. FINITE ELEMENT MODELING AND EXAMPLE 3
The third example presented in this chapter is the cold-formed steel plain
angle columns (Figure 5.7), which Young tested [5.36] and provided
the experimental ultimate loads, load�axial shortening relationships, and
failure modes of the columns. The test program included 24 fixed-ended
cold-formed steel plain angle columns. The test program agrees well with
the criteria previously discussed, in Section 1.3, for a successful experi-
mental investigation. The authors have used the test results to develop a
nonlinear finite element model simulating the buckling behavior of the
columns as detailed by Ellobody and Young [4.9]. The test specimens
were brake-pressed from high strength zinc-coated grades G500 and
G450 structural steel sheets having nominal yield stresses of 500 and
450 MPa, respectively, and conformed to the Australian Standard AS
1397 [5.37]. Each specimen was cut to a specified length of 250, 1000,
1500, 2000, 2500, 3000, and 3500 mm. Three series of plain angles were
tested, having a nominal flange width of 70 mm. The nominal plate
thicknesses were 1.2, 1.5, and 1.9 mm. The three series were labeled
Given: 
Bf =70 mm, t=1.2, 1.5, and1.9 mm, and
L=250–3500 mm 
ri
t 
Bf
Bf
x 
 y 
b 
S S
L 
(A) (B)
Figure 5.7 Example 3 of a fixed-ended cold-formed steel plain angle column [4.9,
5.36]. (A) Fixed-ended plain angle section column. (B) Plain angle section (Section S-S).
90 Finite Element Analysis and Design of Metal Structures
P1.2, P1.5, and P1.9 according to their nominal thickness. The measured
inside corner radius was 2.6 mm for all specimens. The measured cross
section dimensions of the test specimens are detailed by Young [5.36].
The measured flat flange width-to-thickness ratio was 57.9, 45.0, and
35.8 for Series P1.2, P1.5, and P1.9, respectively. The test specimens are
labeled such that the test series and specimen length could be identified
from the label. For example, the label “P1.2L1000” defines the specimen
belonged to test Series P1.2, and the fourth letter “L” indicates the length
of the specimen followed by the nominal column length of the specimen
in millimeters (1000 mm).
The material properties of the flange (flat portion) of the specimens
for each series were determined by tensile coupon tests. The coupons
were taken from the center of the flange plate in the longitudinal direc-
tion of the finished specimens. The coupon dimensions and the tests con-
formed to the Australian Standard AS 1391 [5.38] for the tensile testing
of metals using 12.5 mm wide coupons of gauge length 50 mm. The
Young’s modulus (E), the measured static 0.2% proof stress (σ0.2), the
measured elongation after fracture (ε) based on a gauge length of 50 mm,
and the tensile coupon tests of the flat portions were measured as detailed
by Young [5.36]. The initial overall geometric imperfections of the speci-
mens were measured prior to testing. The maximum overall imperfec-
tions at mid-length were 1/2950, 1/2150, and 1/1970 of the specimen
length for Series P1.2, P1.5, and P1.9, respectively. The measured overall
geometric imperfections of each test specimen are detailed by Young
[5.36]. A servo-controlled hydraulic testing machine was used to apply
compressive axial force to the specimen. The fixed-ended bearings were
designed to restrain against the minor and major axis rotations as well as
twist rotations and warping. Displacement control was used to allow the
tests to be continued in the post-ultimate range. The column tests are
detailed by Young [5.36]. The initial local geometric imperfections, resid-
ual stresses, and corner material properties of the tested plain angle speci-
mens were not reported by Young [5.36]. However, the values of these
measurements are important for finite element analysis. Hence, the initial
local imperfections, residual stresses, and corner material properties of the
angle specimens belonging to the same batched as the column test speci-
mens were measured and reported by Ellobody and Young [4.9].
The finite element program ABAQUS [1.27] was used in the analysis
of plain angle columns tested by Young [5.36]. The model used the mea-
sured geometry, initial local and overall geometric imperfections, residual
91Examples of Finite Element Models of Metal Columns
stresses, and material properties as detailed by Ellobody and Young [4.9].
Since buckling of plain angle columns is very sensitive to large strains, the
S4R element was used in this study to ensure the accuracy of the results.
In order to choose the finite element mesh that provides accurate results
with minimum computational time, convergence studies were conducted.
It is found that 103 10 mm (length by width) ratio provides adequate
accuracy in modeling the flat portions of plain angles while finer mesh
was used at the corner. Following the testing procedures for Series P1.2,
P1.5, and P1.9, the ends of the columns were fixed against all degrees of
freedom except for transitional displacement at the loaded end in the
direction of the applied load. The nodes other than the two ends were
free to translate and rotate in any directions. The load was applied in
increments using the modified Riks method available in the ABAQUS
[1.27] library. The load was applied as static uniform loads at each node
of the loaded end which is identical to the experimental investigation.
The nonlinear geometry parameter (NLGEOM) was included to deal
with the large displacement analysis. The measured stress�strain curves
for flat portions of Series P1.2, P1.5, and P1.9 were used in the analysis.
The material behavior provided by ABAQUS [1.27] allows for a multi-
linear stress�strain curve to be used, as described in Section 3.4.
Cold-formed steel plain angle columns with very high b/t ratio are
likely to fail by pure local buckling. On the other hand, columns with
very low b/t ratio are likely to fail by overall buckling. Both initial local
and overall geometric imperfections are found in columns as a result of
the fabrication process. Hence, superposition of local buckling mode as
well as overall buckling mode with measured magnitudes is recommended
for accurate finite element analysis. These buckling modes can be
obtained by carrying eigenvalue analysis of the column with very high b/t
ratio and very low b/t ratio to ensure local and overall buckling, occurs
respectively. The shape of a local buckling mode as well as overall buck-
ling mode is found to be the lowest buckling mode (eigenmode 1) in the
analysis. This technique is used in this study to model the initial local and
overall imperfections of the columns. Stub columns having very short
length can be modeled for local imperfection only. Since all buckling
modes predicted by ABAQUS [1.27] eigenvalue analysis are generalized
to 1.0, the buckling modes are factored by the measured magnitudes of
the initial local and overall geometric imperfections. Figure 5.8 shows the
unfactored local and overall imperfection buckling modes for angle
specimenP1.9L1500. More details regarding modeling of geometric
92 Finite Element Analysis and Design of Metal Structures
imperfections can be found in Section 4.3. Measured residual stresses are
implemented in the finite element model by using the ABAQUS [1.27]
(�ININTIAL CONDITIONS, TYPE5 STRESS) parameter. The flat
and corner coupons material tests took into consideration of the bending
residual stresses effect, hence, only the membrane residual stresses were
modeled. Detailed information regarding modeling residual stresses can
be found in Section 3.6.
In the verification of the finite element model, a total of 21 cold-
formed steel plain angle columns were analyzed. A comparison between
the experimental results and the results of the finite element model was
carried out. The comparison of the ultimate loads (PTest and PFE), axial
shortening (eTest and eFE) at the ultimate loads, and failure modes obtained
experimentally and numerically are given in Table 5.2. Figure 5.9 plotted
the relationship between the ultimate load and the column effective
length (ley5L/2) for Series P1.2, P1.5, and P1.9, where L is the actual
column length. The column curves show the experimental ultimate loads
Figure 5.8 Initial geometric imperfection modes (eigenmode 1) for plain angle col-
umn P1.9L1500 [4.9]. (A) Local imperfection. (B) Overall imperfection.
93Examples of Finite Element Models of Metal Columns
together with that obtained by the finite element method. It can be seen
that good agreement has been achieved between both results for most of
the columns. The finite element results are slightly higher than that of the
test strengths for Series P1.5 and P1.9. A maximum difference of 15%
was observed between experimental and numerical results for P1.2L2500
column. The mean values of PTest/PFE ratio are 1.00, 0.96, and 0.93 with
the corresponding COV of 0.086, 0.057, and 0.035 for Series P1.2, P1.5,
and P1.9, respectively, as given in Table 5.2. The mean values of eTest/eFE
ratio are 1.09, 1.06, and 1.03 with the COV of 0.111, 0.147, and 0.128
Table 5.2 Comparison between Test and FE Results for Cold-Formed Steel Plain
Angle Columns [4.9]
Specimen
Test FE Test/FE
PTest
(kN)
eTest
(mm)
Failure
Mode
PFE
(kN)
eFE
(mm)
Failure
Mode
PTest
PFE
eTest
eFE
P1.2L250 23.8 0.54 L 24.9 0.61 L 0.96 0.89
P1.2L1000 18.7 1.10 F1 FT 18.1 0.96 F1 FT 1.03 1.14
P1.2L1500 15.2 0.82 F1 FT 15.7 0.70 F1 FT 0.97 1.17
P1.2L2000 12.6 1.66 F1 FT 11.7 1.74 F1 FT 1.08 0.95
P1.2L2500 11.6 1.25 F1 FT 10.1 1.04 F1 FT 1.15 1.20
P1.2L3000 8.0 1.07 F1 FT 8.6 0.98 F 0.93 1.15
P1.2L3500 5.8 1.03 F1 FT 6.4 0.89 F 0.91 1.16
Mean � � � � � � 1.00 1.09
COV � � � � � � 0.086 0.111
P1.5L250 39.6 0.70 L 37.8 0.83 L 1.05 0.84
P1.5L1000 31.0 1.20 F1 FT 31.5 1.39 F1 FT 0.98 0.86
P1.5L1500 25.2 1.25 F1 FT 25.5 1.03 F1 FT 0.99 1.21
P1.5L2000 17.5 1.27 F1 FT 19.7 1.07 F1 FT 0.89 1.19
P1.5L2500 15.7 1.42 F1 FT 16.0 1.19 F1 FT 0.98 1.19
P1.5L3000 13.1 1.32 F1 FT 14.2 1.21 F 0.92 1.09
P1.5L3500 11.5 1.36 F1 FT 12.5 1.29 F 0.92 1.05
Mean � � � � � � 0.96 1.06
COV � � � � � � 0.057 0.147
P1.9L250 57.7 0.80 L 60.6 0.95 L 0.95 0.84
P1.9L1000 47.8 1.40 FT 49.1 1.55 F1 FT 0.97 0.90
P1.9L1500 35.6 1.45 F1 FT 38.4 1.27 F1 FT 0.93 1.14
P1.9L2000 27.1 1.66 F1 FT 30.8 1.45 F1 FT 0.88 1.14
P1.9L2500 22.4 1.88 F1 FT 24.3 1.62 F1 FT 0.92 1.16
P1.9L3000 14.8 1.22 F1 FT 16.7 1.14 F 0.89 1.07
P1.9L3500 14.4 1.15 F1 FT 15.4 1.22 F 0.94 0.94
Mean � � � � � � 0.93 1.03
COV � � � � � � 0.035 0.128
94 Finite Element Analysis and Design of Metal Structures
for Series P1.2, P1.5, and P1.9, respectively. Generally, good agreement
has been achieved for most of the columns. Three modes of failure have
been observed experimentally and verified by the finite element model.
The failure modes are the local buckling (L), flexural buckling (F), and
flexural-torsional buckling (FT).
Figure 5.10 shows the ultimate load against the axial shortening
behavior of column P1.9L2500 that has a length of 2500 mm. The curve
has been predicted by the finite element model and compared with the
test curve. It can be shown that both the column stiffness and behavior
reflect good agreement between experimental and finite element results.
The failure modes observed in the test of P1.9L2500 were interaction of
flexural and flexural-torsional buckling (F1 FT). The same failure mode
has been confirmed numerically by the model shown in Figure 5.11.
0
20
40
60
80
0 500 1000 1500 2000
Effective length, ley (mm)
Lo
ad
, P
 (
kN
)
Test P1.9
FE P1.9 
Test P1.5
FE P1.5 
Test P1.2 
FE P1.2
Figure 5.9 Ultimate loads obtained experimentally and numerically for plain angle
columns for Series P1.2, P1.5, and P1.9 [4.9].
0
10
20
30
0 2 4 6
Shortening (mm)
Lo
ad
 (
kN
)
Test 
FE 
Figure 5.10 Comparison of load�axial shortening curves obtained experimentally
and numerically for column P1.9L2500 [4.9].
95Examples of Finite Element Models of Metal Columns
It can be noticed that the cross section of the column was shifted and
twisted from its undeformed position.
The main design rules used in the study [4.9] are specified in the
AISI [5.39] and the AS/NZS [5.40]. Using the design rules for concen-
trically loaded compression members in the AISI Specification [5.39] and
AS/NZS [5.40], the nominal axial strength (Pn) were calculated as follows:
Pn5AeFn ð5:1Þ
where Ae is the effective area and Fn is the critical buckling stress. The
critical buckling stress (Fn) is calculated as follows:
Fn5 ð0:658λ2
c ÞFy for λc # 1:5 ð5:2Þ
Fn 5
0:877
λ2
c
� �
Fy for λc . 1:5 ð5:3Þ
where λc is the nondimensional slenderness calculated as follows:
λc5
ffiffiffiffiffi
Fy
Fe
r
ð5:4Þ
Fixed end
Axial shortening
Undeformed position
Loaded end
Deformed position 
Figure 5.11 Failure mode and undeformed position of column P1.9L2500 [4.9].
96 Finite Element Analysis and Design of Metal Structures
where Fy is the yield stress which is equal to the 0.2% proof stress (σ0.2)
and Fe is the least of the elastic flexural, torsional, and flexural-torsional
buckling stress determined in accordance with Sections C4.1�C4.3 of
the AISI Specification and Sections 3.4.1�3.4.4 of the AS/NZS.
Young [5.36] concluded that the design strengths obtained using the
AISI Specification and AS/NZS for the tested cold-formed steel plain
angle columns are generally quite conservative. Hence, Eqs (5.2) and
(5.3) have been modified as follows:
Fn5 ð0:5λ2
c ÞFy for λc # 1:4 ð5:5Þ
Fn5
0:5
λ2
c
� �
Fy for λc. 1:4 ð5:6Þ
where the slenderness (λc) is calculated as that in Eq. (5.4) with the
exception that the elastic buckling stress (Fe) is determined from the flex-
ural buckling only in accordance with Section C4.1 of the AISI
Specification and Section 3.4.2 of the AS/NZS. The column design
strength (PP) proposed by Young [5.36] was then computed as PP5AeFn.
It has been shown that the design strengths obtained using the proposed
Eqs (5.5) and (5.6) compared well with the test strengths conducted by
Young [5.36].
After the verification of the finite element model, parametric studies
were carried out to study the effects of cross section geometries on the
strength and behavior of angle columns. A total of 35 plain angle columns
were analyzed in the parametric study. Five series of column P0.8, P1.0,
P2.6, P4.2, and P10.0 having plate thickness of 0.8, 1.0, 2.6, 4.2, and
10.0 mm, respectively were studied. All angle sections had the overall
flange width of 70 mm which is having the same flange width as the test
specimens. The five series had the flat flange width-to-thickness ratio (b/t)
of 85, 65, 25, 15, and 5 for Series P0.8, P1.0, P2.6, P4.2, and P10.0,
respectively. Each series of columns consists of seven column lengths of
250, 1000, 1500, 2000, 2500, 3000, and 3500 mm. The maximum initial
local geometric imperfection magnitude was taken as the measured value
of 0.14% of the plate thickness. The maximum initial overall geometricimperfection magnitude was taken as the average of the measured maxi-
mum overall imperfections of the tested series which is equal to L/2360,
where L is the column length.
97Examples of Finite Element Models of Metal Columns
The results of the parametric study were compared with the nominal
(unfactored) design strengths obtained using the AISI Specification and
AS/NZS as well as compared with the design strengths obtained using
the equations proposed by Young [5.36]. Figures 5.12�5.16 show a com-
parison between the finite element results (PFE) with the nominal (unfac-
tored) design strengths (Pn) obtained using the AISI Specification and
AS/NZS, the design strengths (PF) that consider flexural buckling only
when calculating the elastic buckling stress (Fe), and the design strengths
(PP) proposed by Young [5.36]. The column curves are nondimensiona-
lized with respect to the nominal stub column design strength (section
0.0
0.5
1.0
1.5
0 40 80 120 160 200
le / ry
P
 / 
P
s
Pn (AISI and AS/NZS)
PFE
PF (Flexural buckling)
PP (Young′s equation)
Figure 5.12 Comparison of FE results with predicted design strengths for Series P0.8
(b/t5 85) [4.9].
0.0
0.5
1.0
1.5
0 40 80 120 160 200
le / ry
P
 / 
P
s
Pn (AISI and AS/NZS)
PFE
PF (Flexural buckling)
PP (Young′s equation)
Figure 5.13 Comparison of FE results with predicted design strengths for Series P1.0
(b/t5 65) [4.9].
98 Finite Element Analysis and Design of Metal Structures
capacity) Ps, i.e., Ps5AeFy, where Ae is the effective area at yield stress of
the flat portion (Fy) as shown on the vertical axis of Figures 5.12�5.16.
The horizontal axis is plotted as le/ry, where le is the effective length that
assumed equal to one-half of the column length and ry is the radius of
gyration about the minor principal y-axis. It can be seen that the AISI
and AS/NZS design strengths (Pn) are generally quite conservative for
angle columns with b/t ratios of 85, 65, and 25 as shown in
Figures 5.12�5.14. On the other hand, the AISI and AS/NZS design
strengths overestimated the column strengths for most of the columns
that have b/t ratios of 15 and 5, as shown in Figures 5.15 and 5.16. The
0.0
0.5
1.0
1.5
0 40 80 120 160 200
le / ry
P
 / 
P
s
Pn (AISI and AS/NZS)
PF (Flexural buckling)
P FE 
PP (Young′s equation)
Figure 5.14 Comparison of FE results with predicted design strengths for Series P2.6
(b/t5 25) [4.9].
0.0
0.5
1.0
1.5
0 40 80 120 160 200
le / ry
P
 / 
P
s
Pn (AISI and AS/NZS)
PF (Flexural buckling)
PFE 
PP (Young′s equation)
Figure 5.15 Comparison of FE results with predicted design strengths for Series P4.2
(b/t5 15) [4.9].
99Examples of Finite Element Models of Metal Columns
design strengths (PF) that consider flexural buckling only overestimated
the column strengths of all b/t ratios. Good agreement has been achieved
between FE results and the design strengths (PP) obtained using the equa-
tion proposed by Young [5.36] for most of the columns.
5.6. FINITE ELEMENT MODELING AND EXAMPLE 4
The fourth example presented in this chapter is the cold-formed stainless
steel circular hollow section columns (Figure 5.17), which were tested by
Young and Hartono [5.20], and they provided the experimental ultimate
loads, load�axial shortening relationships, and failure modes of the col-
umns. The test program included 16 fixed-ended cold-formed stainless
steel circular hollow section columns. The test program agrees well with
the criteria discussed in Section 1.3 for a successful experimental investiga-
tion. The authors have used the test results to develop a nonlinear finite
element model simulating the buckling behavior of the columns as detailed
by Young and Ellobody [5.15]. Three series (Series C1, C2, and C3) of cir-
cular hollow section columns were tested. The test specimens were cold-
rolled from annealed flat strips of type 304 stainless steel. Each specimen
was cut to a specified length (L) ranging from 550 to 3000 mm. The mea-
sured cross section dimensions of the test specimens are detailed by Young
and Hartono [5.20]. The Series C1, C2, and C3 had an average measured
outer diameter (D) of 89.0, 168.7, and 322.8 mm and an average thickness
(t) of 2.78, 3.34, and 4.32 mm, respectively. The average measured outer
0.0
0.5
1.0
1.5
0 40 80 120 160 200
le / ry
P
 / 
P
s
Pn (AISI and AS/NZS)
PF (Flexural buckling)
PFE
PP (Young′s equation)
Figure 5.16 Comparison of FE results with predicted design strengths for Series
P10.0 (b/t5 5) [4.9].
100 Finite Element Analysis and Design of Metal Structures
diameter-to-thickness (D/t) ratio is 32.0, 50.5, and 74.7 for Series C1, C2,
and C3, respectively. The test specimens are labeled such that the test series
and specimen length could be identified from the label. For example, the
label “C1L1000” defines the specimen belonged to test Series C1, and the
letter “L” indicates the length of the specimen followed by the nominal
column length of the specimen in millimeters (1000 mm).
The material properties of each series of specimens were determined
by tensile coupon tests. The coupons were taken from the untested speci-
mens at 90� from the weld in the longitudinal direction. The coupon
dimensions and the tests conformed to the Australian Standard AS 1391
[5.38] for the tensile testing of metals using 12.5 mm wide coupons of
gauge length 50 mm. The Young’s modulus (E0), the measured static
0.2% proof stress (σ0.2), the measured elongation after fracture based on a
gauge length of 50 mm were measured as detailed in Ref. [5.20]. The ini-
tial overall geometric imperfections of the specimens were measured prior
to testing. The average values of overall imperfections at mid-length were
1/1715, 1/3778, and 1/3834 of the specimen length for Series C1, C2,
and C3, respectively. The measured overall geometric imperfections for
each test specimen are detailed by Young and Hartono [5.20]. The initial
local geometric imperfections of the tested cold-formed stainless steel circu-
lar hollow section columns were not reported by Young and Hartono [5.20].
Given:
D = 100–200 mm, t=1 mm, and
L=500–3500 mm 
L 
(A) (B)
D 
t 
Slender section 
S S 
Figure 5.17 Example 4 of a fixed-ended cold-formed stainless steel circular hollow
section column [5.15,5.20]. (A) Fixed-ended slender circular hollow section. (B) Slender
circular hollow section (section S-S).
101Examples of Finite Element Models of Metal Columns
However, the values of the initial geometric imperfections are important
for finite element analysis. Hence, the initial local geometric imperfections
of the stainless steel circular hollow section specimen belonging to the
same batch as the column test specimens are measured in this study and
reported by Young and Ellobody [5.15]. A cold-formed stainless steel
circular hollow section test specimen of 250 mm in length of Series C1
was used for the measurement of local imperfections. The maximum
magnitude of local plate imperfection was 0.089 mm, which is equal to
3.2% of the plate thickness of the specimen belonged to Series C1. The
same factor was used to predict the initial local geometric imperfections for
Series C2 and C3.
The finite element program ABAQUS [1.27] was used to investigate
the buckling behavior of the cold-formed stainless steel slender circular
hollow section columns. The tests conducted by Young and Hartono
[5.20] were modeled using the measured geometry, initial local and overall
geometric imperfections, and material properties. In order to choose the
finite element mesh that provides accurate results with minimum computa-
tional time, convergence studies were conducted. It is found that the mesh
size around 103 10 mm (length by width) provides adequate accuracy and
minimum computational time in modeling the cold-formed stainless steel
circular hollow section columns. Following the testing procedures for
Series C1, C2, and C3, the ends of the columns werefixed against all
degrees of freedom except for the displacement at the loaded end in the
direction of the applied load. The nodes other than the two ends were free
to translate and rotate in any directions. The load was applied in increments
using the modified Riks method available in the ABAQUS library [1.27].
The load was applied as static uniform loads at each node of the loaded end
using displacement control which is identical to the experimental investi-
gation. The nonlinear geometry parameter (�NLGEOM) was included
to deal with the large displacement analysis. The measured stress�strain
curves of Series C1, C2, and C3 were used in the analysis. The material
behavior provided by ABAQUS [1.27] allows for a multilinear stress�strain
curve to be used, as described in Section 3.4.
Cold-formed stainless steel columns with large D/t ratio are likely to
fail by local buckling or interaction of local and overall buckling depend-
ing on the column length and dimension. Both initial local and overall
geometric imperfections were found in the tested columns. Hence, super-
position of local buckling mode as well as overall buckling mode with
measured magnitudes is recommended in the finite element analysis.
102 Finite Element Analysis and Design of Metal Structures
These buckling modes can be obtained by carrying eigenvalue analyses of
the column with large D/t ratio as well as small D/t ratio to ensure local
and overall buckling occurs, respectively. Only the lowest buckling mode
(eigenmode 1) was used in the eigenvalue analyses. This technique was
used in this study to model the initial local and overall imperfections of
the columns. Since all buckling modes predicted by ABAQUS [1.27]
eigenvalue analysis are normalized to 1.0, the buckling modes were fac-
tored by the measured magnitudes of the initial local and overall geomet-
ric imperfections. Figure 5.18 shows the local and overall imperfection
buckling modes for specimen C2L1500. More details regarding modeling
of geometric imperfections can be found in Section 4.3.
The cold-formed stainless steel circular hollow section columns tested
by Young and Hartono [5.20] were used to verify the finite element
model. The comparison of the ultimate loads (PTest and PFE) and axial
shortening (eTest and eFE) at the ultimate loads obtained experimentally
Figure 5.18 Initial geometric imperfection modes (eigenmode 1) for stainless cold-
formed steel circular hollow section specimen C2L1500 [5.15]. (A) Local imperfection.
(B) Overall imperfection.
103Examples of Finite Element Models of Metal Columns
and numerically are given in Table 5.3. It can be seen that good agree-
ment has been achieved between both results for most of the columns.
The mean value of PTest/PFE ratio is 0.98 with the corresponding COVof
0.016, as given in Table 5.3. The mean value of eTest/eFE ratio is 0.99
with the COV of 0.095. Three modes of failure have been observed
experimentally and confirmed numerically by the finite element analysis.
The failure modes were yielding failure (Y), local buckling (L), and flex-
ural buckling (F). Figure 5.18 shows the applied load against the axial
shortening behavior of column specimen C3L1000 that has an outer
diameter of 322.8 mm and a length of 1000 mm. The curve has been pre-
dicted using the finite element analysis and compared with the test curve.
There has been generally good agreement between experimental and
finite element results. Figure 5.19 shows the deformed shape of column
specimen C2L2000 observed experimentally and numerically using the
FE analysis. The column has an outer diameter of 168.7 mm and a length
of 2000 mm. The failure modes observed in the test were interaction of
Table 5.3 Comparison between Test and Finite Element Results for Cold-Formed
Stainless Steel Circular Hollow Section Columns [5.15,5.20]
Specimen
Test FE Test/FE
PTest
(kN)
eTest
(mm)
PFE
(kN)
eFE
(mm)
Failure
Mode
PTest
PFE
eTest
eFE
C1L550 235.2 16.88 240.5 15.41 Y 0.98 1.10
C1L1000 198.4 10.26 206.8 10.89 Y 0.96 0.94
C1L1500 177.4 5.77 181.8 6.54 F 0.98 0.88
C1L2000 165.1 4.83 167.9 5.54 F 0.98 0.87
C1L2500 151.6 5.39 148.9 5.93 F 1.02 0.91
C1L3000 133.4 4.99 134.5 5.41 F 0.99 0.92
C2L550 495.6 9.41 522.0 8.32 Y 0.95 1.13
C2L1000 474.9 14.64 486.7 13.03 L 0.98 1.12
C2L1500 461.0 15.92 468.9 15.25 L1 F 0.98 1.04
C2L2000 431.6 13.32 443.7 15.11 L1 F 0.97 0.88
C3L1000 1123.9 8.05 1140.0 7.93 Y 0.99 1.02
C3L1500 1119.7 14.38 1130.0 13.12 Y 0.99 1.10
C3L2000 1087.8 14.53 1100.0 14.90 L 0.99 0.98
C3L2500 1045.7 19.12 1070.0 18.05 L 0.98 1.06
C3L3000 1009.5 15.64 1040.0 16.74 L 0.97 0.93
Mean � � � 0.98 0.99
COV � � � 0.016 0.095
104 Finite Element Analysis and Design of Metal Structures
local and flexural buckling (L1 F). It can be seen that the finite element
model accurately predicted the failure modes observed in the test.
After the verification of the finite element model developed in Ref. [5.15],
parametric studies were performed to study the effect of local buckling
on the strength and behavior of the slender circular hollow section col-
umns. A total of 42 columns were analyzed in the parametric study. The
columns are labeled such that the outer diameter and column length
could be identified from the label. For example, the label “C100L1000”
defines the circular hollow section column using a letter “C” followed
by the value of the outer diameter in millimeters (100 mm) and the letter
“L” indicates the length of the column followed by the column length
in millimeters (1000 mm). Six series of slender circular hollow sections
(Series C100, C120, C140, C160, C180, and C200) having the outer
diameter of 100, 120, 140, 160, 180, and 200 mm, respectively, and a
plate thickness of 1.0 mm were studied. The Series C100, C120, C140,
C160, C180, and C200 had the outer diameter-to-thickness ratio (D/t)
of 100, 120, 140, 160, 180, and 200, respectively. Each series of columns
consists of seven column lengths of 500, 1000, 1500, 2000, 2500,
3000, and 3500 mm. The maximum initial local geometric imperfection
magnitude was taken as the measured value of Series C1 which is equal
to 3.2% of the plate thickness. The initial overall geometric imperfection
magnitude was taken as the average of the measured overall imperfections
of the Series C1 which is equal to L/1715, where L is the column length.
The measured stress�strain curve of Series C1 was used in the parametric
study.
0
300
600
900
1200
0 4 8 12 16
Axial shortening (mm)
Lo
ad
 (
kN
)
Test
FE
Figure 5.19 Load�axial shortening curves obtained experimentally and numerically
for column C3L1000 [5.15].
105Examples of Finite Element Models of Metal Columns
The design rules specified in the ASCE [5.17] are based on the Euler
column strength that requires the calculation of tangent modulus (Et) using an
iterative design procedure. The design rules specified in the EC3 [5.19] are
based on the Perry curve that needs only the initial Young’s modulus (E0)
and a number of parameters to calculate the design stress. The design rules
specified in the AS/NZS [5.18] adopt either the Euler column strength or
alternatively the Perry curve; the latter is used in this paper. The fixed ended
columns were designed as concentrically loaded compression members and
the effective length (le) were taken as one-half of the column length (le5L/2)
as recommended by Young and Rasmussen [5.41]. In the three specifications,
the effective area (Ae) is to account for local buckling of slender sections.
5.6.1 American Specification
The nominal (unfactored) design strength for concentrically loaded cylindrical
tubular compression members in the ASCE [5.17] is calculated as follows:
PASCE5FnAe ð5:7Þ
The flexural buckling stress (Fn) that account for overall buckling is
calculated as follows:
Fn5
π2Et
ðle=rÞ2
#Fy ð5:8Þ
where Et is the tangent modulus determined using Eq. (B-2) of the ASCE,
le is the effectively length,r is the radius of gyration of the full cross section,
and Fy is the yield stress that is equal to the static 0.2% proof stress (σ0.2).
The effective area (Ae) that accounts for local buckling is calculated as
follows:
Ae5 12 12
Et
E0
	 
2 !
12
A0
A
	 
" #
A ð5:9Þ
where E0 is the initial Young’s modulus, A is the full cross-sectional area,
and A0 is the reduced cross-sectional area which is determined as follows:
A05KcA#A for
D
t
#
0:881E0
Fy
ð5:10Þ
and
Kc 5
ð12CÞðE0=FyÞ
ð8:932λcÞðD=tÞ 1
5:882C
8:932λc
ð5:11Þ
106 Finite Element Analysis and Design of Metal Structures
where C is the ratio of effective proportional limit-to-yield strength as
given in Table A17 of the ASCE [5.17], λc5 3.084C with a limiting
value of (E0/Fy)/(D/t), D is the outer diameter, and t is the plate thick-
ness of the stainless steel tube.
5.6.2 Australian New/Zealand Standard
The unfactored design strength for concentrically loaded cylindrical tubular
compression members in the AS/NZS [5.18] is calculated using the Perry
curve as follows:
PAS=NZS5FnAe ð5:12Þ
where
Fn 5
Fy
ϕ1
ffiffiffiffiffiffiffiffiffiffiffiffiffiffiffiffi
ϕ22λ2
p #Fy ð5:13Þ
ϕ5 0:5ð11 η1λ2Þ ð5:14Þ
η5α λ2λ1ð Þβ 2λ0
� �
$ 0 ð5:15Þ
λ5
le
r
ffiffiffiffiffiffiffiffiffiffi
Fy
π2E0
r
ð5:16Þ
The parameters α, β, λ0, and λ1 required for the calculation of the
AS/NZS design strengths were calculated from the equations proposed by
Rasmussen and Rondal [5.42]. The columns investigated in the paramet-
ric study had slenderness (λ) ranged from 0.043 to 0.06 calculated using
Eq. (5.16), which covered the short to intermediate column slenderness.
Hence, the results of the present study are limited to cold-formed stainless
steel slender circular hollow sections for short to intermediate column
slenderness. The effective area (Ae) is calculated in the same way as the
ASCE [5.17], except for the reduction factor Kc as given in Eq. (5.11). In
the AS/NZS [5.18], the reduction factor Kc is calculated as follows:
Kc 5
ð12CÞðE0=FyÞ
ð3:2262λcÞðD=tÞ 1
0:178C
3:2262λc
ð5:17Þ
107Examples of Finite Element Models of Metal Columns
5.6.3 European Code
The unfactored design strength for concentrically loaded cylindrical tubular
compression members in the EC3 [5.19] is calculated as follows:
PEC35χFyAe ð5:18Þ
where
χ5
1
ϕ1
ffiffiffiffiffiffiffiffiffiffiffiffiffiffiffiffi
ϕ22λ
2
q # 1 ð5:19Þ
ϕ5 0:5ð11αðλ2λ0Þ1λ
2Þ ð5:20Þ
λ5
le
r
ffiffiffiffiffiffiffiffiffiffi
FyβA
π2E0
s
ð5:21Þ
βA5
1 for Class 1; 2; or 3 cross sections
Ae
A
for Class 4 cross sections
8<
: ð5:22Þ
The values of the imperfection factor α and limiting slenderness λ0
can be obtained from Table 5.2 of the EC3 [5.19].
The effective area (Ae) is taken as the full area (A) for Class 1 (D/t# 50ε2),
Class 2 (D/t# 70ε2), and Class 3 (D/t# 90ε2) cross sections, where ε is
calculated as follows:
ε5
ffiffiffiffiffiffiffiffiffiffiffiffiffiffiffiffiffiffiffiffiffiffiffiffi
235
Fy
E0
210; 000
s
ð5:23Þ
It should be noted that the EC3 [5.19] does not provide design rules
for the calculation of effective area (Ae) for Class 4 (D/t. 90ε2) slender
circular hollow sections. In this study, the circular hollow sections investi-
gated in the parametric study are classified as Class 4 slender sections, but
no design provision is given in the EC3 for the calculation of the effective
area. Hence, the full cross-sectional area (A) was used.
108 Finite Element Analysis and Design of Metal Structures
5.6.4 Proposed Design Equation
In this study, effective area equation for cold-formed stainless steel slender
circular hollow section columns was proposed. The proposed effective
area equation for Class 4 slender circular hollow sections is as follows:
Ae5Aε
125
D=t
	 
0:1
ð5:24Þ
where A is the full cross-sectional area, ε is calculated from Eq. (5.23),
D is the outer diameter, and t is the plate thickness of the circular stainless
steel tube.
The proposed design strength for concentrically loaded cylindrical
tubular compression members can be calculated in the same way as the
EC3 [5.19]:
PP5χFy Ae ð5:25Þ
where χ is the reduction factor for flexural buckling that is calculated in
the same way as in Eq. (5.19), Fy is the yield stress that is equal to the
static 0.2% proof stress (σ0.2), and Ae is the proposed effective area as
given in Eq. (5.20).
5.6.5 Comparison of Column Strengths
The column strengths predicted from the parametric study were com-
pared with the unfactored design strengths calculated using the American
(ASCE [5.17]), Australian/New Zealand (AS/NZS [5.18]), and European
(EC3 [5.19]) specifications for cold-formed stainless steel structures.
The measured material properties obtained from the tensile coupon of
Series C1, which is the same material properties as those used in the
parametric study, were used to calculate the design strengths. The column
strength ratios for all specimens are shown on the vertical axis of
Figures 5.20�5.25, while the horizontal axis is plotted against the effec-
tive length (le) that is assumed equal to one-half of the column length.
Figures 5.20 and 5.21 show that the design strengths calculated using the
AS/NZS and EC3 specifications are unconservative for the columns hav-
ing D/t ratios of 100 and 120, except for the short columns with lengths
of 500 and 1000 mm. The design strengths calculated using the American
Specification and the proposed design equation are generally conservative,
except for some long columns. Figures 5.22�5.25 show that the design
strengths calculated using the AS/NZS and EC3 specifications are
109Examples of Finite Element Models of Metal Columns
generally unconservative for cold-formed stainless steel slender circular
hollow section columns having D/t ratios of 140, 160, 180, and 200,
while the ASCE is quite conservative. The design strengths predicted
using the proposed design equation are generally conservative for
Figure 5.20 Comparison of experimental analysis (A) and finite element analysis (B)
failure modes for specimen C2L2000 [5.16].
0.0
0.2
0.4
0.6
0.8
1.0
1.2
1.4
0 500 1000 1500 2000
Effective length, le (mm)
P
F
E
/P
D
es
ig
n
Proposed
ASCE
AS/NZS
EC3
Figure 5.21 Comparison of FE strengths with design strengths for Series C100, [5.15].
110 Finite Element Analysis and Design of Metal Structures
0.0
0.2
0.4
0.6
0.8
1.0
1.2
1.4
0 500 1000 1500 2000
Effective length, le (mm)
P
F
E
/P
D
es
ig
n
Proposed
ASCE
AS/NZS
EC3
Figure 5.22 Comparison of FE strengths with design strengths for Series C120 [5.15].
0.0
0.2
0.4
0.6
0.8
1.0
1.2
1.4
0 500 1000 1500 2000
Effective length, le (mm)
P
F
E
/P
D
es
ig
n
Proposed
ASCE
AS/NZS
EC3
Figure 5.23 Comparison of FE strengths with design strengths for Series C140 [5.15].
0.0
0.2
0.4
0.6
0.8
1.0
1.2
1.4
0 500 1000 1500 2000
Effective length, le (mm)
P
F
E
/P
D
es
ig
n
Proposed
ASCE
AS/NZS
EC3
Figure 5.24 Comparison of FE strengths with design strengths for Series C160 [5.15].
111Examples of Finite Element Models of Metal Columns
cold-formed stainless steel slender circular hollow section columns having
D/t ratios of 140, 160, 180, and 200.
REFERENCES
[5.1] Schmidt, H. Stability of steel shell structures. General report. Journal of
Constructional Steel Research, 55(1), 159�181, 2000.
[5.2] Galambos, T. V. Guide to stability design criteria for metal structures. New York,
NY: John Wiley & Sons, 1988.
[5.3] ANSYS Inc.. ANSYS 5.4-Manual: Theory, elements and commands references.
USA, 1998.
[5.4] Schmidt, H. and Krysik, R. Towards recommendations for shell stability design by
means of numerically determined buckling loads, In: Jullien, J. F., editor. Buckling
of shell structures, on land, in the sea and in the air, Proc. Int. Coll. Lyon, London/
New York: Elsevier Applied Science, 508�519, 1991.
Proposed
ASCE
AS/NZS
EC3
0.0
0.2
0.4
0.6
0.8
1.0
1.2
1.4
0 500 1000 1500 2000
Effective length, le (mm)
P
F
E
/P
D
es
ig
n
Figure 5.25 Comparisonof FE strengths with design strengths for Series C180 [5.15].
Proposed
ASCE
AS/NZS
EC3
0.0
0.2
0.4
0.6
0.8
1.0
1.2
1.4
0 500 1000 1500 2000
Effective length, le (mm)
P
F
E
/P
D
es
ig
n
Figure 5.26 Comparison of FE strengths with design strengths for Series C200 [5.15].
112 Finite Element Analysis and Design of Metal Structures
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref1
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref1
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref1
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref2
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref2
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref3
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref3
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref4
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref4
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref4
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref4
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref4
[5.5] EC3. Eurocode 3: Design of steel structures Part 1-6: Strength and stability of shell
structures. London, UK: British Standards Institution, BS EN 1993-1-6, 2007.
[5.6] Narayanan, S. and Mahendran, M. Ultimate capacity of innovative cold-formed
steel columns. Journal of Constructional Steel Research, 59(4), 489�508, 2003.
[5.7] Schafer, B. W. and Peköz, T. Computational modeling of cold-formed steel:
Characterizing geometric imperfections and residual stresses. Journal of Constructional
Steel Research, 47(3), 193�210, 1998.
[5.8] Kwon, Y. B. and Hancock, G. J. A nonlinear elastic spline finite strip analysis for
thin-walled sections. Thin-Walled Structures, 12(4), 295�319, 1991.
[5.9] Raftoyiannis, I. G. and Ermopoulos, J. C. Stability of tapered and stepped steel
columns with initial imperfections. Engineering Structures, 27(8), 1248�1257,
2005.
[5.10] EC3. Eurocode 3: Design of steel structures Part 1-1: General rules and rules for
buildings. London, UK: British Standards Institution, BS EN 1993-1-1, 2005.
[5.11] Spyrakos, C. C. and Raftoyiannis, I. G. Linear and nonlinear finite element analy-
sis. Pittsburgh, PA: Algor Publishing Division, 1998.
[5.12] Zhu, J. H. and Young, B. Aluminum alloy tubular columns—Part I: Finite element
modeling and test verification. Thin-Walled Structures, 44(9), 961�968, 2006.
[5.13] Yan, J. and Young, B. Numerical investigation of channel columns with com-
plex stiffeners—Part I: Tests verification. Thin-Walled Structures, 42(6), 883�893,
2004.
[5.14] Mazzolani, F. M. Aluminum alloy structures. 2nd ed., London: E & FN Spon, 1995.
[5.15] Young, B. and Ellobody, E. Column design of cold-formed stainless steel slender cir-
cular hollow sections. Steel and Composite Structures, 6(4), 285�302, 2006.
[5.16] Ellobody, E. and Young, B. Investigation of cold-formed stainless steel non-slender
circular hollow section columns. Steel and Composite Structures, 7(4), 321�337,
2007.
[5.17] ASCE. Specification for the design of cold-formed stainless steel structural mem-
bers. Reston, Virginia: American Society of Civil Engineers, SEI/ASCE-02, 2002.
[5.18] AS/NZS. Cold-formed stainless steel structures. Australian/New Zealand
Standard. Sydney, Australia: Standards Australia, AS/NZS 4673:2001, 2001.
[5.19] EC3. Eurocode 3: Design of steel structures—Part 1.4: General rules—
Supplementary rules for stainless steels. CEN, Brussels: European Committee for
Standardization, ENV 1993-4, 1996.
[5.20] Young, B. and Hartono, W. Compression tests of stainless steel tubular members.
Journal of Structural Engineering, ASCE, 128(6), 754�761, 2002.
[5.21] L. Gardner, A new approach to structural stainless steel design. PhD thesis.
London: Department of Civil and Environmental Engineering, Imperial College
of Science, Technology and Medicine, 2002.
[5.22] Ellobody, E. Buckling analysis of high strength stainless steel stiffened and unstif-
fened slender hollow section columns. Journal of Constructional Steel Research,
63(2), 145�155, 2006.
[5.23] Zhang, Y., Wang, C. and Zhang, Z. Tests and finite element analysis of pin-ended
channel columns with inclined simple edge stiffeners. Journal of Constructional
Steel Research, 63(3), 383�395, 2007.
[5.24] Becque, J. and Rasmussen, K. J. R. A numerical investigation of local-overall
interaction buckling of stainless steel lipped channel columns. Journal of
Constructional Steel Research, 65(8-9), 1685�1693, 2009.
[5.25] Gao, L., Sun, H., Jin, F. and Fan, H. Load-carrying capacity of high-strength steel
box-sections I: Stub columns. Journal of Constructional Steel Research, 65(4),
918�924, 2009.
113Examples of Finite Element Models of Metal Columns
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref5
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref5
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref6
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref6
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref6
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref7
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref7
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref7
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref7
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref8
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref8
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref8
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref9
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref9
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref9
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref9
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref10
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref10
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref11
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref11
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref12
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref12
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref12
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref13
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref13
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref13
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref13
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref14
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref15
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref15
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref15
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref16
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref16
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref16
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref16
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref17
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref17
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref18
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref18
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref19
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref19
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref19
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref20
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref20
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref20
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref21
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref21
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref21
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref21
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref22
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref22
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref22
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref22
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref23http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref23
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref23
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref23
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref24
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref24
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref24
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref24
[5.26] AISI. Specification for the design of cold-formed steel structural members.
Washington, DC, 1996.
[5.27] Theofanous, M. and Gardner, L. Testing and numerical modelling of lean duplex
stainless steel hollow section columns. Engineering Structures, 31(12), 3047�3058,
2009.
[5.28] Gardner, L. and Nethercot, D. A. Numerical modeling of stainless steel structural
components: A consistent approach. Journal of Structural Engineering ASCE, 130
(10), 1586�1601, 2004.
[5.29] Ashraf, M., Gardner, L. and Nethercot, D. A. Finite element modelling of struc-
tural stainless steel cross-sections. Thin-Walled Structures, 44(10), 1048�1062,
2007.
[5.30] Goncalves, R. and Camotim, D. Geometrically non-linear generalised beam theory
for elastoplastic thin-walled metal members. Thin-Walled Structures, 51, 121�129,
2012.
[5.31] Goncalves, R. and Camotim, D. Generalised beam theory-based finite elements
for elastoplastic thin-walled metal members. Thin-Walled Structures, 49(10),
1237�1245, 2011.
[5.32] Zhu, J. H. and Young, B. Test and design of aluminum alloys compression mem-
bers. Journal of Structural Engineering, 132(7), 1096�1107, 2006.
[5.33] The Aluminum Association. Aluminum design manual. Washington, DC: The
Aluminum Association, 2005.
[5.34] AS/NZS. Aluminum structures—Part 1: Limit state design, Australian/New
Zealand Standard AS/NZS 1664.1:1997. Sydney, Australia: Standards Australia,
1997.
[5.35] EC9. Eurocode 9: Design of aluminum structures—Part 1-1: General rules—
General rules and rules for buildings. Final Draft October 2000. European
Committee for Standardization, DD ENV 1999-1-1:2000, 2000.
[5.36] Young, B. Tests and design of fixed-ended cold-formed steel plain angle columns.
Journal of Structural Engineering, ASCE, 130(12), 1931�1940, 2004.
[5.37] Australian Standard. Steel sheet and strip—hot-dipped zinc-coated or aluminum/
zinc-coated, AS 1397. Sydney, Australia: Standards Association of Australia, 1993.
[5.38] Australian Standard. Methods for tensile testing of metals, AS 1391. Sydney,
Australia: Standards Association of Australia, 1991.
[5.39] American Iron and Steel Institute (AISI). Specification for the design of cold-
formed steel structural members. Washington, DC: AISI, 1996.
[5.40] Australian/New Zealand Standard (AS/NZS). Cold-formed steel structures.
Sydney, Australia: Standards Australia, AS/NZS 4600:1996, 1996.
[5.41] Young, B. and Rasmussen, K. J. R. Tests of fixed-ended plain channel columns.
Journal of Structural Engineering, ASCE, 124(2), 131�139, 1998.
[5.42] Rasmussen, K. J. R. and Rondal, J. Strength curves for metal columns. Journal of
Structural Engineering ASCE, 113(6), 721�728, 1997.
114 Finite Element Analysis and Design of Metal Structures
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref25
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref25
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref26
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref26
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref26
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref26
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref27
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref27
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref27
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref27
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref28
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref28
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref28
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref28
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref29
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref29
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref29
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref29
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref30
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref30
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref30
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref30
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref31
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref31
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref31
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref32
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref32
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref33
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref33
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref33
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref34
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref34
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref34
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref35
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref35
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref36
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref36
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref37
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref37
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref38
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref38
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref39
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref39
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref39
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref40
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref40
http://refhub.elsevier.com/B978-0-12-416561-8.00005-6/sbref40
CHAPTER66
Examples of Finite Element
Models of Metal Beams
6.1. GENERAL REMARKS
This chapter presents examples of different finite element models of metal
beams based on the background of finite element analysis as detailed in
Chapters 1�4. The examples presented in this chapter are already pub-
lished in journal papers. The examples are arbitrary, chosen from research
conducted by the authors of this book so that all related information
regarding the finite element models developed in the papers can be
provided to readers. The chosen finite element models are for beams
constructed from different metals having different mechanical properties,
cross sections, boundary conditions, and geometries. Once again, when
presenting the previously published models developed for metal beams,
the main objective is not to repeat the previously published information
but to explain the fundamentals of the finite element method used in
developing the models.
This chapter starts with a review of recently published finite element
models on metal beams. After that, the chapter presents three examples of
finite element models on metal beams previously published by the
authors. The authors also highlight how the information presented in the
previous chapters is used to develop the examples of finite element
models as discussed in the current chapter. The experimental investiga-
tions simulated, finite element models developed, verifications of finite
element models, results obtained, and comparisons with design values in
current specifications are presented in this chapter with clear references.
The authors have an aim that the presented examples highlighted in this
chapter can explain to readers the effectiveness of finite element models
in providing detailed data that augment experimental investigations
conducted on metal beams. The results are discussed to show the
significance of the finite element models in predictingthe structural
response of metal beams.
115
Finite Element Analysis and Design of Metal Structures
DOI: http://dx.doi.org/10.1016/B978-0-12-416561-8.00006-8
© 2014 Elsevier Inc.
All rights reserved.
http://dx.doi.org/10.1016/B978-0-12-416561-8.00006-8
6.2. PREVIOUS WORK
Many finite element models were developed in the literature. Some of these
models with detailed examples are presented in the following paragraphs for
the investigations of the behavior and design of metal beams. The aforemen-
tioned numerical investigations were performed on metal beams constructed
from steel, cold-formed steel, stainless steel, and aluminum alloy materials.
Liu and Chung [6.1] have investigated the structural performance of steel
beams with large web openings and various shapes and sizes through finite
element analysis. The study has looked into the Vierendeel mechanism in
steel beams with web opening and the empirical interaction formulae
presented in current codes of practice. The finite element analysis detailed in
the study [6.1] included steel beams with web openings of various shapes
and sizes. The study has shown that all steel beams with large web openings
of various shapes behave similarly under a wide range of applied moments
and shear forces. It was also shown that the failure modes were common in
all beams and the yield patterns of those perforated sections at failure are sim-
ilar. The authors have performed parametric studies using finite element
method, which yielded a simple empirical design method applicable for per-
forated sections with web openings of various shapes and sizes. The authors
have used isoparametric 8-node shell element (see Section 3.2). The stresses
incorporated in each shell element include two in-plane direct stresses, one
in-plane shear stress, and two out-of-plane shear stresses. The material
nonlinearity (see Section 4.4) was incorporated into the finite element
model. A bilinear stress�strain curve was adopted in the material modeling
of steel together with the von Mises yield criteria and nonassociate plastic
flow rule (see Section 3.4). It should be noted that in order to model load
redistribution after yielding, elastic unloading was also incorporated. The
geometric nonlinearity (see Section 4.5) was also incorporated into the finite
element model, with large deformation in the perforated section after yield-
ing may be predicted accurately to allow for load redistribution within the
perforated sections. This allowed the Vierendeel mechanism with the
formation of plastic hinges in the tee-sections above and below the web
openings to be investigated in detail. The authors have found that the finite
element modeling produced good comparisons with laboratory tests on steel
beams with circular web openings having diameter of 0.60 times the overall
height of the beam (h), which is subjected to significant moment�shear
interaction [6.2,6.3]. It was concluded that the finite element models are
considered to be applicable in the present study to perforated sections with
116 Finite Element Analysis and Design of Metal Structures
various shapes and sizes. The developed finite element model [6.1] was used
to perform parametric studies.
Mohri et al. [6.4] have performed a combined theoretical and numeri-
cal stability analyses of unrestrained mono-symmetric thin-walled beams.
The study discussed a contribution to the overall stability of unrestrained
thin-walled elements with open sections. The authors have developed a
nonlinear finite element model for beam lateral buckling stability analysis.
The authors have looked into the EC3 [5.10] approach and performed
analytical solutions for checking the stability of laterally unrestrained
beams. The analytical solutions were discussed in the study [6.4] and
compared against finite element results. The general-purpose finite
element software ABAQUS [1.27] was used in numerical simulations.
Three-dimensional beam elements with warping (B31OS) and shell ele-
ments (S8R5) (see Section 3.2) were chosen in modeling the lateral
buckling phenomena. The authors have found that the analytical results
were close to shell element results. The authors have found that shell ele-
ments could consider local buckling, section distortion, and the local
effects of concentrated loads and boundary conditions, which were all
ignored in the beam element theory.
Zhu and Young [6.5] have conducted a combined experimental and
numerical investigation of aluminum alloy flexural members. The investi-
gations were performed on different sizes of square hollow sections sub-
jected to pure bending. Material properties of each specimen were also
measured. The authors have developed a nonlinear finite element model,
which was verified against the pure bending tests. The verified finite ele-
ment model was used to perform parametric studies on aluminum alloy
beams of square hollow sections. The experimental and numerical
bending strengths were compared against the design strengths calculated
using the American [5.33], Australian/New Zealand [5.34], and
European [5.35] specifications for aluminum structures. The bending
strengths were also compared with the design strengths predicted by the
direct strength method, which was developed for cold-formed carbon
steel members. The authors have proposed design rules for aluminum
alloy square hollow section beams based on the current direct strength
method. In addition, reliability analysis was performed to evaluate the
reliability of the design rules. The general-purpose finite element soft-
ware ABAQUS [1.27] was used in the analysis for the simulation of
aluminum alloy beams subjected to pure bending. Residual stresses were
not included in the model. This is because in extruded aluminum alloy
117Examples of Finite Element Models of Metal Beams
profiles, residual stresses have very small values. For practical purpose,
these have a negligible effect on load-bearing capacity as recommended
by Mazzolani [5.14]. The authors have modeled only one half of the
beam due to symmetry (see Section 3.3). The displacement control loading
method was used, which is identical to that used in the beam tests. The
load was applied in increments using the Riks method (see Section 4.6)
with automatic increment size being applied. The material nonlinearity or
“plasticity” was included in the finite element model. The general-purpose
shell elements (S4R) were used in the finite element model. The authors
have conducted convergence studies to choose the finite element mesh that
provides accurate results with minimum computational time. It was found
that when meshing each side of the cross section with 10 elements, the
results will be accurate compared with the tests.
Liu and Gannon [6.6] have presented the results of a finite element
study on the behavior and capacity of W-shape steel beams reinforced
with welded plates under loading. The authors have developed a nonlin-
ear finite element model, which was verified against published test results
by one of the authors [6.7]. The verified model was used to conduct
parametric studies investigating the effects of reinforcing patterns, preload
magnitudes at the time of welding, and initial imperfections of the unre-
inforced beam. The study [6.6] has shown that the increase in the preload
magnitude at the time of reinforcing resulted in a reduction in the ulti-
mate capacity of reinforced beams failing by lateral torsional buckling
(LTB). The finite element model was developed using the general-
purpose finite element software ANSYS [5.3] to simulate a flexural
member under a four-point loading with reinforcing plates added at
various load levels. The beam cross section, weld, and reinforcing plates
were all modeled using Shell 181 element as specified in ANSYS [5.3].
This 3D, 4-node element is suitable for the analysis of thin to moderately
thick structures with large rotation and largestrain nonlinearities and also
capable of buckling simulation (see Section 3.2). Considering the symme-
try of specimen geometry and loading, only half of a specimen was mod-
eled. Convergence studies were carried out by the authors to choose the
best finite element mesh. It was found that a mesh size of 103 20 mm
was selected for flanges and reinforcing plate and a mesh size of
153 20 mm was used for the web. Bearing plates at the loading points
and end supports were modeled using the Solid 45 brick element to allow
the load to be distributed across the width of the flanges. Solid 45 is a
3D, 8-node structural solid element capable of including effects of large
118 Finite Element Analysis and Design of Metal Structures
deflection, large strain, and stress stiffening (see Section 3.2). The effect of
initial geometric imperfections on unreinforced steel beams was investi-
gated in the study [6.6]. Also, residual stresses were incorporated into the
finite element models at two different stages. The initial residual stress for
the beam section alone was transformed into a series of discrete uniform
stresses that could be applied to each element in the model. These resid-
ual stresses were then specified by creating an initial stress field applied to
the model during the first substep of the first load step of the analysis. At
the second stage of the analysis, the residual stresses in the reinforcing
plates and in the beam section due to welding were added after the beam
had reached the specified preload magnitude. Since the initial stress file
may only be input in the first load step, residual stresses at the second
stage were introduced alternatively by specifying a temperature body force
on the shell elements. A similar technique was used by Wu and Grondin
[6.8]. In the nonlinear analysis, a Newton�Raphson procedure (see
Chapter 4) was used to perform equilibrium iterations until convergence
criteria were satisfied. Loads were applied to the model over a load step
which was divided into a number of substeps to obtain an accurate
solution.
Theofanous and Gardner [6.9] have reported material and three-point
bending tests on lean duplex stainless steel hollow section beams. The
three-point bending tests were simulated by finite element analysis.
The validated model was used to perform parametric studies to assess the
effects of cross section aspect ratio, cross section slenderness, and moment
gradient on the strength and deformation capacity of lean duplex stainless
steel beams. Based on both the experimental and numerical results, the
authors have proposed slenderness limits and design rules for incorpo-
ration into structural stainless steel design standards. The authors have
used the general-purpose finite element software ABAQUS [1.27] to
develop the models. The initial geometric imperfections, material proper-
ties, and mesh density were investigated by the authors. The reduced
integration 4-node doubly curved general-purpose shell element S4R
with finite membrane strains (see Section 3.2) has been used to simulate
the structural behavior of the lean duplex stainless steel beams. The
element has been previously used by the authors [6.10,6.11] and shown
to perform well in the modeling of thin-walled metallic structures. Mesh
convergence studies (see Section 3.3) were performed by the authors to
evaluate the best mesh that provides accurate results with reasonable
computational time. Only half of the cross section of each specimen was
119Examples of Finite Element Models of Metal Beams
modeled due to symmetry. The load was applied as a point load at the
junction of the web with the corner radius in the lower (tension) part of
the beam to avoid web crippling. The authors have used the measured
geometry and material properties in the finite element models. Due to
the absence of global buckling, only local geometric imperfections have
been incorporated in the finite element models in the form of the lowest
buckling mode shape. A linear eigenvalue buckling analysis (see
Section 4.3) was therefore initially conducted using the subspace iteration
method for eigenmode extraction. Subsequently, a geometrically and
materially nonlinear analysis (see Sections 4.4 and 4.5) incorporating geo-
metric imperfections was carried out. The modified Riks method (see
Section 4.6) was employed in the nonlinear analyses.
Sweedan [6.12] has numerically investigated the lateral stability of
cellular steel beams. Three-dimensional finite element modeling was
presented for simply supported I-shaped cellular steel beams having differ-
ent cross-sectional dimensions, span lengths, and web perforation config-
urations. The author has performed stability analyses for beams subjected
to equal end moments, mid-span concentrated loads, and uniformly dis-
tributed loads. The study has shown that the moment gradient coefficient
was considerably affected by the beam geometry, slenderness, and web
perforation configuration. Based on the study [6.12], a simplified
approach was developed to enable accurate prediction of a moment mod-
ification factor for cellular beams. It was shown that the proposed
approach allows for accurate and conservative evaluation of the critical
moment associated with the lateral torsional�distortional buckling of
cellular beams. The study also has presented several numerical examples
to illustrate the application of the proposed procedure. The 3D finite
element model for I-shaped cellular steel beams was developed using the
general-purpose finite element software ANSYS [5.3]. The 4-node shell
element (Shell 181), which has six degrees of freedom at each node
including three translations and three rotations, was used. Numerical
computations were conducted for cellular steel beams that were assumed
to be constructed of linear elastic material. Convergence studies were per-
formed to choose the best finite element mesh that provides accurate
results with less computational time.
Haidarali and Nethercot [6.13] have developed two series of finite
element models investigating the buckling behavior of laterally restrained
cold-formed steel Z-section beams. The developed models have
accounted for the nonlinear material and geometry. The first series of the
120 Finite Element Analysis and Design of Metal Structures
models allowed for the possibility of combined local�distortional
buckling, and the second series of models allowed for local buckling only.
The authors have used previously published four-point bending tests to
verify the finite element models. The general-purpose finite element soft-
ware ABAQUS [1.27] has been used to perform the nonlinear analyses.
The finite element results compared well against the tests. The general-
purpose shell elements S4R were used for all the components of the finite
element models. The initial geometric imperfections were included in the
models. The authors have performed an elastic eigenvalue buckling
analysis to obtain appropriate eigenmodes for local and distortional buck-
ling. These buckling modes were inserted into the nonlinear analysis to
define the shape and distribution of initial imperfections. The authors
have found some difficulties for the local buckling mode for some
sections as the pure local buckling modes for these sections were obtained
at very high eigenmodes, which required considerable computational
time. Therefore, it was decided to generate the shape and distribution of
initial imperfections manually with the aid of the finite strip software
CUFSM [6.14]. The classical finite strip method uses polynomial func-
tions for the deformed shape in the transverse direction, while a single
half sine wave is used for the longitudinal shape function.
Ellobody [6.15] has investigated the behavior of normal and high
strength castellated steel beams under combined lateral torsional and dis-
tortional buckling modes. An efficient nonlinear 3D finiteelement model
has been developed for the analysis of the beams. The initial geometric
imperfections and material nonlinearities were carefully considered in the
analysis. The nonlinear finite element model was verified against tests on
castellated beams having different lengths and different cross sections.
Failure loads and interaction of buckling modes as well as load�lateral
deflection curves of castellated steel beams were investigated in this study.
The author has performed parametric studies to investigate the effects of
the cross section geometries, beam length, and steel strength on the
strength and buckling behavior of castellated steel beams. The study
[6.15] has shown that the presence of web distortional buckling (WDB)
causes a considerable decrease in the failure loads of slender castellated
steel beams. It was also shown that the use of high strength steel offers a
considerable increase in the failure loads of less slender castellated steel
beams. The failure loads predicted from the finite element model were
compared with that predicted from Australian Standards [6.16] for steel
beams under LTB. It was shown that the Specification predictions are
121Examples of Finite Element Models of Metal Beams
generally conservative for normal strength castellated steel beams failed by
LTB, but unconservative for castellated steel beams failed by WDB, and
quite conservative for high strength castellated steel beams failed by LTB.
The general-purpose finite element software ABAQUS [1.27] was used
to perform the finite element analyses. The author has performed an
eigenvalue buckling analysis, which was followed by a nonlinear
load�displacement analysis. The material and geometric nonlinearities
were included in the analyses. The author has used a combination of
4-node and 3-node doubly curved shell elements with reduced integra-
tion (S4R and S3R). Convergence studies were performed to choose the
finite element mesh that provides accurate results with minimum
computational time. It was found that approximately 153 15 mm (length
by width of S4R element and depth by width of S3R element) provides
adequate accuracy in modeling the web, while a finer mesh of approxi-
mately 83 15 mm was used in the flange. The initial geometric
imperfections were included in the analyses.
Ellobody [6.17] has extended the study [6.15] to discuss the nonlinear
analysis of normal and high strength cellular steel beams under combined
buckling modes. The author has developed a nonlinear 3D finite element
model, which accounted for the initial geometric imperfections, residual
stresses, and material nonlinearities of flange and web portions of cellular
steel beams. The nonlinear finite element model was verified against tests
on cellular steel beams having different lengths, cross sections, loading
conditions, and failure modes. Failure loads, load�mid-span deflection
relationships, and failure modes of cellular steel beams were predicted
from the finite element analysis. The author has performed parametric
studies involving 120 cellular steel beams using the verified finite element
model to study the effects of the cross section geometries, beam length,
and steel strength on the strength and buckling behavior of cellular steel
beams. The study [6.17] has shown that cellular steel beams failed by
combined web distortional and web-post buckling (WPB) modes
exhibited a considerable decrease in the failure loads. It was also shown
that the use of high strength steel offers a considerable increase in the fail-
ure loads of less slender cellular steel beams. The failure loads predicted
from the finite element model were compared with that predicted from
Australian Standards [6.16] for steel beams under LTB. It was shown that
the specification predictions are generally conservative for normal strength
cellular steel beams failed by LTB, but unconservative for cellular steel
beams failed by combined web distortional and WPB, and quite
122 Finite Element Analysis and Design of Metal Structures
conservative for high strength cellular steel beams failed by LTB. The
general-purpose finite element software ABAQUS [1.27] was used to per-
form the finite element analyses. The author has performed an eigenvalue
buckling analysis, which was followed by a nonlinear load�displacement
analysis. Both material and geometric nonlinearities were included in the
analyses. The author has used a combination of 4-node and 3-node
doubly curved shell elements with reduced integration (S4R and S3R).
Convergence studies were performed to choose the finite element mesh
that provides accurate results with minimum computational time. It was
found that approximately 403 50 mm (length by width of S4R element
and depth by width of S3R element) provides adequate accuracy in
modeling the web, while a mesh of approximately 353 50 mm was used
in the flange. The initial geometric imperfections and residual stresses
were included in the analyses.
Anapayan and Mahendran [6.18] have presented the performance of
LiteSteel Beam (LSB), which is a new hollow flange channel section
developed using a patented dual electric resistance welding and cold-
forming process. The beam has a unique geometry consisting of torsion-
ally rigid rectangular hollow flanges and a slender web, and is commonly
used as flexural members. The authors have shown that the LSB flexural
members are subjected to a relatively new lateral distortional buckling
mode, which reduces their moment capacities. Therefore, a detailed
investigation into the lateral buckling behavior of LSB flexural members
was undertaken by the authors using experiments and finite element
analyses. This study has presented the finite element models developed to
simulate the behavior and capacity of LSB flexural members subjected to
lateral buckling. The models have included material inelasticity, lateral
distortional buckling deformations, web distortion (WD), residual stresses,
and geometric imperfections. The study [6.18] included a comparison of
the finite element ultimate moment capacities with predictions from other
numerical analyses and available buckling moment equations as well as
experimental results. It was shown that the developed finite element
models accurately predicted the behavior and moment capacities of LSBs.
The validated model was then used to perform parametric studies, which
produced accurate moment capacity data for all the LSB sections and
improved design rules for LSB flexural members subjected to lateral dis-
tortional buckling. The general-purpose finite element software
ABAQUS [1.27] was used to perform the analyses. The shell element
S4R5 was used to develop the LSB model. Convergence studies were
123Examples of Finite Element Models of Metal Beams
performed to predict the best finite element mesh that provides accurate
results with less computational time. It was shown that a minimum mesh
size density comprising 53 10 mm elements was required to represent
accurate residual stress distributions, spread of plasticity, and local buckling
deformations of LSBs. Element widths less than or equal to 5 mm and a
length of 10 mm were selected as the suitable mesh size. Nine integration
points through the thickness of the elements were used to model the dis-
tribution of flexural residual stresses in the LSB sections and the spread of
plasticity through the thickness of the shell elements, as recommended by
Kurniawan and Mahendran [6.19].
Zhou et al. [6.20] have investigated the performance of aluminum
alloy plate girders subjected to shear force through numerical investiga-
tion. The aluminum alloy plate girders were fabricated by welding of
three plates to form an I-section. The authors have developed a nonlinear
finite element model, which was verified against experimental results.
The geometric and material nonlinearities were included in the finite
element model. The welding of thealuminum plate girders and the influ-
ence of the heat-affected zone (HAZ) were included in the finite element
model. The ultimate loads, web deformations, and failure modes of
aluminum plate girders were predicted from the study. The authors have
performed parametric studies investigating the effects of cross section
geometries and the web slenderness on the behavior and shear strength of
aluminum alloy plate girders. The shear resistances obtained from the
study [6.20] were compared against the design strengths predicted using
the European Code [5.35] and American Specifications [5.33] for alumi-
num structures. Based on the study, the authors have proposed a design
method to predict the shear resistance of aluminum alloy plate girders by
modifying the design rules specified in the European Code [5.35]. The
general-purpose finite element software ABAQUS [1.27] was used in the
analysis for the simulation of aluminum alloy plate girders subjected to
shear force. The material nonlinearity or plasticity was included in the
finite element model. The general-purpose shell elements S4R were used
in the finite element model. The authors have conducted convergence
studies to choose the finite element mesh that provides accurate results
with minimum computational time. It was found that a mesh size of
83 8 mm (length by width) in the HAZ area and a mesh size of
153 15 mm elsewhere provided accurate results compared with the tests.
Soltani et al. [6.21] have developed a numerical model to predict the
behavior of castellated beams with hexagonal and octagonal openings.
124 Finite Element Analysis and Design of Metal Structures
The material and geometric nonlinearities were considered in the model.
The authors have performed an eigenvalue buckling analysis to model the
initial geometric imperfections. The finite element model was verified
against previously published experimental results. The ultimate loads and
general failure modes were predicted from the study. The numerical
results have been compared with those obtained from the design method
presented in the EC3 [5.10]. The general-purpose finite element software
LUSAS [6.22] was used to perform the finite element analyses. The webs,
flanges, intermediate plates, and stiffeners of the castellated steel beams
were modeled by a 3D 8-node thin shell element QSL8 available in the
LUSAS [6.22] element library. The element has three translational degrees
of freedom at each of four corners and four mid-sides and normal rota-
tions at the two Gauss points along each side. Only one layer of elements
was used through thickness direction. Finer meshes were generated to
model areas near the openings in order to improve precision and accom-
modate the opening shapes. Only half of the beam was modeled owing
to symmetry to reduce the model size and subsequent processing time.
Although the cross section was also symmetrical about its major and
minor axes, it was necessary to model the full cross section because the
buckled shape is nonsymmetrical. The regular meshing was employed for
all components of the beam. The density and the configuration of the
finite element mesh were determined based on results obtained from con-
vergence studies in order to provide a reasonable balance between
accuracy and computational expense. The dimensions of elements with
the minimum width, located around the opening, were chosen to ensure
the aspect ratio was kept below 5. The nonlinear analyses were performed
with meshes varying from 1472 to 3776 elements. The geometric nonlin-
earity was considered to account for the large displacements. The geo-
metrically nonlinear analysis followed the continually changing geometry
of the beam when formulating each successive load increment.
Kankanamge and Mahendran [6.23] have highlighted the importance
of cold-formed steel beams as floor joists and bearers in buildings. The
authors have undertaken finite element analyses to investigate the LTB
behavior of simply supported cold-formed steel lipped channel beams
subjected to uniform bending. The general-purpose finite element soft-
ware ABAQUS [1.27] was used to develop the finite element model,
which was verified using available numerical and experimental results.
The validated finite element model was used to perform parametric
studies to simulate the LTB behavior and capacity of cold-formed steel
125Examples of Finite Element Models of Metal Beams
beams under varying conditions. The authors have compared the
moment capacity results against the predictions from the current design
rules in many cold-formed steel codes, and suitable recommendations
were made. The authors have found that European design rules [6.24]
were conservative, while Australian/New Zealand [6.25] and North
American [6.26] design rules were unconservative. Therefore, the authors
have proposed design equations for the calculation of the moment capac-
ity based on the available finite element analysis results. This study [6.23]
has presented the details of the parametric study, recommendations to the
current design rules, and the new design rules proposed in this research
for LTB of cold-formed steel lipped channel beams.
6.3. FINITE ELEMENT MODELING AND RESULTS OF
EXAMPLE 1
The first example presented in this chapter is the simply supported
castellated beams constructed from carbon steel modeled by Ellobody
[6.15]. The castellated steel beams were subjected to distortional buckling
and tested by Zirakian and Showkati [6.27] (Figure 6.1). The castellated
(B)(A)
Middle symmetry
surface
Support stiffener
Figure 6.1 Comparison of experimental (B) and numerical (A) buckled shapes at fail-
ure for castellated steel beam specimen having a depth of 210 mm and a length of
4400 mm [6.15,6.27].
126 Finite Element Analysis and Design of Metal Structures
beams were loaded with central concentrated load. Lateral deflections
were prevented at mid-span and near the supports using lateral bracing.
The testing program included six full-scale beam tests having different
cross section geometries and lengths as detailed in Ref. [6.27]. The castel-
lated beam tests were designed so that the top compression flange of the
beam was restrained against lateral buckling at mid-span and near the
supports. Hence, the cross section at quarter-span was subjected to unre-
strained distortional buckling, while the cross section at mid-span was
subjected to restrained distortional buckling. The two buckling modes are
detailed in [6.27,6.28]. The load was applied step-by-step until failure
occurred. Failure was identified when the lateral deflections were large at
quarter-span locations and unloading took place. The material properties
of flange and web portions were determined from tensile coupon tests as
detailed in Ref. [6.27]. The test program provided useful and detailed
data regarding the behavior of castellated steel beams and conformed to
the criteria of a successful experimental investigation highlighted in
Section 1.3.
The tests carried out by Zirakian and Showkati [6.27] were modeled
by Ellobody [6.15] using the general-purpose finite element software
ABAQUS [1.27]. The model has accounted for the measured geometry,
initial geometric imperfections, and measured material properties of
flange and web portions. The finite element analyses of the castellated
steel beams comprised linear eigenvalue buckling analysis (see
Section 4.3) as well as materially and geometrically nonlinear analyses
detailed in Sections 4.4 and 4.5, respectively. A combination of 4-node
and 3-node doubly curved shell elements with reduced integration (S4R
and S3R) were used to model the flanges and web of the castellated steel
beams (see Section 3.2). In order to choose the finite element mesh that
provides accurate results with minimum computational time, convergence
studies (see Section 3.3) were conducted. It was found that approximately
153 15 mm (length bywidth of S4R element and depth by width of
S3R element) provides adequate accuracy in modeling the web, while a
finer mesh of approximately 83 15 mm was used in the flange. Only half
of the castellated beam was modeled due to symmetry (see Section 3.3).
The load was applied in increments as concentrated static load, which
was also identical to the experimental investigation.
The stress�strain curve for the structural steel given in the EC3 [5.10]
was adopted in the study [6.15] with measured values of the yield stress
and ultimate stress used in the tests [6.27]. The material behavior
127Examples of Finite Element Models of Metal Beams
provided by ABAQUS [1.27] (using the PLASTIC option) allows a
nonlinear stress�strain curve to be used (see Section 3.4). Buckling of
castellated beams depends on the lateral restraint conditions to
compression flange and geometry of the beams. Two main buckling
modes detailed in Refs [6.27,6.28] could be identified as unrestrained and
restrained lateral distortional buckling modes. The lateral distortional
buckling modes could be obtained by performing eigenvalue buckling
analysis (see Section 4.3) for castellated beams with actual geometry and
lateral restraint conditions to the compression flange. Only the first buck-
ling mode (eigenmode 1) was used in the eigenvalue analysis. Since
buckling modes predicted by ABAQUS eigenvalue analysis [1.27] are
generalized to 1.0, the buckling modes were factored by a magnitude of
Lu/1000, where Lu is the length between points of effective bracing. The
factored buckling modes were inserted into the load�displacement nonlin-
ear analysis of the castellated beams following the eigenvalue prediction. It
should be noted that the investigation of castellated beams with different
slenderness ratios could result in LTB mode with or without WDB mode.
Hence, the eigenvalue buckling analysis must be performed for each castel-
lated beam with actual geometry to ensure that the correct buckling mode
could be incorporated in the nonlinear displacement analysis.
The finite element model for castellated beams under distortional buck-
ling developed by Ellobody [6.15] was verified against the test results detailed
in Ref. [6.27]. The failure loads, failure modes, and load�lateral deflection
curves obtained experimentally and numerically using the finite element
model were compared. The failure loads obtained from the tests as well as
calculated using the design equation proposed in Ref. [6.29] as reported in
Ref. [6.27] (PTest/Calculated) and finite element analyses performed in Ref.
[6.15] (PFE) were compared. The mean value of PTest/Calculated/PFE ratio is
1.01 with the coefficient of variation (COV) of 0.020. Three failure modes
were observed experimentally [6.27] and verified numerically [6.15] using
the finite element model. All the tested castellated beams [6.27] underwent
LTB and WD, while steel beam yielding (SY) was observed in castellated
beams with lengths of 3600 and 4400 mm. The SY failure mode was
predicted from the finite element model by comparing the von Mises stresses
in the castellated beams at failure against the measured yield stresses. On the
other hand, the SY failure mode was judged in the tests by comparing the
test failure loads against the plastic collapse loads (Ppx) calculated according
to AS4100 [6.16]. The load�lateral deflection curves predicted experimen-
tally and numerically were compared as shown in Figure 6.2. The curves
128 Finite Element Analysis and Design of Metal Structures
were plotted as an example at quarter-span of test specimen C180-3600 at
the top, middle, and bottom points of the web of castellated beam. It was
shown that good agreement was generally achieved between experimental
and numerical results. The positive sign represents the lateral deflection in
front of the web and the negative sign represents the lateral deflection at
back of the web. The deformed shapes of castellated beams at failure
observed experimentally and numerically were also compared. Figure 6.1
showed as an example of the buckled shape of specimen C210-4400
observed in the test in comparison with that predicted from the finite
element analysis. It was shown that the experimentally and numerically
deformed shapes are in good agreement. The failure mode observed
experimentally and confirmed numerically was a combination of LTB, WD,
and SY. The data obtained from ABAQUS [1.27] has shown that the von
Mises stresses at the maximum stressed fibers at the top and bottom flanges at
mid-span exceeded the measured yield stresses.
The verified finite element model developed in Ref. [6.15] was used
to study the effects of the cross section geometries, beam length, steel
strength, and nondimensional slenderness on the strength and buckling
behavior of castellated steel beams. A total of 96 castellated steel beams
were analyzed using the finite element model. The dimensions and mate-
rial properties of the castellated steel beams were reported in Ref. [6.15].
The investigated castellated steel beams had different nondimensional
slenderness (λ) calculated based on AS4100 [6.16] ranged from 1.0 to 3.1.
The nondimensional slenderness (λ) is equal to the square root of the
major axis full plastic moment divided by the elastic buckling moment,
0
5
10
15
20
25
–2 0 2 4 6 8
Lateral deflection (mm)
Lo
ad
 (
kN
)
FE (Top)
Test (Middle)
Test (Bottom)
FE (Bottom)
FE (Middle)
Test (Top)
Figure 6.2 Comparison of load�lateral deflection curves at quarter-span of castellated
steel beam specimen having a depth of 180 mm and a length of 3600 mm [6.15].
129Examples of Finite Element Models of Metal Beams
which was considered as a guide for beam slenderness in the study. The
failure loads and failure modes of the castellated steel beams were
predicted from the parametric studies as reported in Ref. [6.15]. The
study [6.15] has shown that the failure loads of the castellated beams
showed logical and expected results, with less slender beams followed a
more “plastic collapse” mode, which are obviously driven by the steel
strength. The more slender the beam, the more elastic buckling will be
obtained. Furthermore, the collapse behavior is dependent on the lateral
torsional and WDB behavior of the beam. It was also shown that the use
of high strength steel offered a considerable increase in the failure loads of
less slender castellated steel beams.
The plastic collapse load (Ppx) and the design failure load (PAS4100)
calculated according to AS4100 [6.16] were obtained in the study [6.15].
The failure loads obtained from the parametric study (PFE) were com-
pared against the design failure loads calculated using the AS4100 [6.16]
(PAS4100) for the castellated steel beams. The study [6.15] has shown that
the specification predictions were generally conservative for the castellated
beams failed by LTB and having steel yield stress of 275 MPa. The
specification predictions were unconservative for the beams failed mainly
by WD. The specification predictions were also unconservative for the
beams failed by combined (LTB1 SY1WD) and (LTB1WD). On the
other hand, the specification predictions were quite conservative for all
remaining castellated steel beams, particularly those fabricated from high
strength steel. The failure loads of castellated steel beams predicted from
the finite element analysis (PFE) and design guides (PAS4100) were nondi-
mensionlized with respect to the plastic collapse load (Ppx) and plotted
against the nondimensional flange width-to-thickness ratio (B/t) in
Figure 6.3 as reported in Ref. [6.15]. The comparison of the numerical
and design predictions has shown that the AS4100 design guide was gen-
erally conservative for the castellated steel beams with normal yield stres-
ses, while it was quite conservative for the beams with higher yield
stresses.
6.4. FINITE ELEMENT MODELING AND RESULTS OF
EXAMPLE 2
Thesecond example presented in this chapter is the beams constructed
from aluminum alloy carried out by Zhu and Young [6.5], which pro-
vided the experimental bending strengths, moment-curvature curves, and
130 Finite Element Analysis and Design of Metal Structures
failure modes of the aluminum alloy beams. A nonlinear finite element
model was developed to simulate the flexural behavior of the beams based
on the test results as described in Ref. [6.5]. The tested beams [6.5] had
square hollow sections and were subjected to pure bending (Figure 6.4).
The test specimens were fabricated by extrusion using high strength
6061-T6 heat-treated aluminum alloys. The test program included 10
simply supported beams, which is detailed in Ref. [6.5] and, once again,
no intention to repeat the materials published in this paper. However, it
should be mentioned that the experimental program presented was
planned such that 10 beam tests were accurately investigated. The tests
were well instrumented such that the experimental results were used in
the verification of the finite element models developed by Zhu and
Young [6.5]. Material properties of each specimen were determined by
longitudinal tensile coupon tests. Hinge and roller supports were
simulated by half round and pin, respectively. The simply supported
specimens were loaded symmetrically at two points to the bearing plates
within the moment span using a spreader beam. Half round and pin were
also used at the loading points. Stiffening plates were used at the loading
points and supports to prevent web bearing failure at the load of concen-
tration. The experimental ultimate moments (MExp) were obtained using
half of the ultimate applied load from the actuator multiplied by the lever
arm (distance from the support to the loading point) of the specimens.
0
0.2
0.4
0.6
0.8
1
0 4 8 12 16 20 24 28 32 4036
B/t
P
F
E
/P
px
 a
nd
 P
A
S
41
00
/P
px
FE (G1)
AS4100 (G2)
FE (G3)
AS4100 (G3)
AS4100 (G1)
FE (G2)
Figure 6.3 Comparison of finite element analysis and design predictions for castel-
lated steel beams in groups G1�G3 having a depth of 180 mm and a length of
5200 mm with different steel grades [6.15].
131Examples of Finite Element Models of Metal Beams
The mass of the spreader beam, half round, pin, bearing plates, and stiff-
ening plates were included in the calculation of the ultimate moments.
The observed failure modes included local buckling (L) and material
yielding (Y).
The general-purpose finite element program ABAQUS [1.27] was
used in the study [6.5] for the simulation of aluminum alloy beams sub-
jected to pure bending. Residual stresses were not included in the model.
Only half of the beam was modeled by using symmetric condition at
mid-length of the specimen. The midpoint of the bottom flange at mid-
length was restrained for longitudinal degree of freedom to avoid the sin-
gularity of the stiffness matrix. The displacement control loading method
was used in the finite element model, which is identical to that used in
the beam tests. The load was applied to the beam by specifying a displace-
ment to the reference point of the rigid surface at the loading point. The
(A)
Mid span
(B)
Figure 6.4 Comparison of experimental (A) and finite element (B) analysis failure
modes of aluminum alloy beam of square hollow section 1533 1533 3 [6.5].
132 Finite Element Analysis and Design of Metal Structures
default Riks method (see Section 4.6) with automatic increment size was
applied. The measured material properties of the test specimens were
used in the finite element model. The material nonlinearity or plasticity
was included in the finite element model using a mathematical model
known as the incremental plasticity model available in the ABAQUS
[1.27] library. The model was based on the centerline dimensions of the
cross sections. The general-purpose shell elements S4R (see Section 3.2)
were used in the finite element model. In order to choose the finite ele-
ment mesh that provides accurate results with minimum computational
time, mesh sensitivity and convergence studies were carried out in this
study. Generally, each cross section was meshed into 10 elements.
The finite element model developed by the authors [6.5] was verified
against the experimental results presented in the same paper [6.5]. The
finite element model was also verified against three pure bending test
results reported by Zhu and Young [6.30]. The ultimate moments and
failure modes predicted by the finite element analysis were compared
with the experimental results [6.5,6.30]. It was shown that the ultimate
moments (MFEA) obtained from the finite element model are generally in
good agreement with the experimental ultimate moments (MExp). The
mean value of the experimental-to-numerical ultimate moment ratio
(MExp/MFEA) was 0.98 with the corresponding COV of 0.044, as pre-
sented in Ref. [6.5]. The failure modes at ultimate moment obtained
from the tests and finite element analysis for each specimen were also
compared in Ref. [6.5]. The observed failure modes included local buck-
ling (L) and material yielding (Y) due to large deflection. The failure
modes predicted by the finite element analysis were in good agreement
with those observed in the tests. Figure 6.4A showed a photograph of
specimen H-1533 1533 3 after the ultimate moment has been reached.
The specimen failed by local buckling at mid-span. Figure 6.4B showed
the deformed shape of the same specimen predicted by the finite element
analysis after the ultimate moment has been reached. Figure 6.5 shows a
comparison of the moment-curvature curves obtained from the test and
predicted by the finite element analysis for specimen H-763 763 3. It was
shown that the finite element analysis curve followed the experimental
curve closely, except that the moments predicted by the finite element
analysis were slightly higher than the experimental moments in the
nonlinear region.
The verified finite element model was used to perform parametric
studies, which included 60 beam specimens of square hollow sections
133Examples of Finite Element Models of Metal Beams
with different geometries and aluminum alloy strengths. The nominal
flexural strengths (unfactored design strengths) predicted by the American
Specification [5.33] (MAA), Australian/New Zealand Standard [5.34]
(MAS/NZS), and European Code [5.35] (MEC9) for aluminum structures,
as well as the current direct strength method [6.31] (MDSM) and the
modified direct strength method [6.32] (MDSM-M) were compared with
the bending strengths obtained from the parametric study (MFEA) and
experimental program (MExp) in the study [6.5]. Figure 6.6 shows a com-
parison of numerical (MFEA) and experimental (MExp) results, which were
nondimensionlized with respect to the design strengths (Mn) calculated
5
6
7
4
3
2
1
0
0 0.1 0.2
FEA
ExperimentalB
en
di
ng
 m
om
en
t (
kN
.m
)
k (10–3/mm)
0.3
Figure 6.5 Comparison of experimental and numerical moment-curvature curves for
specimen H-763 763 3 [6.5].
2
1
0
0 50 100 150
Flange slenderness, b/t
200 300250
AA
AS/NZS
EC9
DSM
DSM-M
M
F
E
A
/M
n 
an
d 
M
E
xp
/M
n
Figure 6.6 Comparison of experimental and numerical data with design strengths
(Mn) [6.5].
134 Finite Element Analysis and Design of Metal Structures
using the American, Australian/New Zealand, and European
Specifications for aluminum structures, as well as the current direct
strength method and the modified direct strength method, against the
nondimensional flange slenderness ratio (b/t) for aluminum beams. It was
shown that the predictions given by the modified direct strength method
were in best agreement with the numerical and test results. Hence, the
modified direct strength method was recommended for the design of alu-
minum alloy flexural members of square hollow sections subjected to
bending.
6.5. FINITE ELEMENT MODELING AND RESULTS OF
EXAMPLE3
The third example presented in this chapter is the simply supported cellu-
lar steel beams constructed from carbon steel modeled by Ellobody
[6.17], shown in Figures 6.7 and 6.8. The full-scale destructive tests on
simply supported cellular steel beams were conducted by Surtees and Liu
[6.33], Warren [6.34], Tsavdaridis and D’Mello [6.35], and Tsavdaridis
et al. [6.36]. The test specimens were denoted C1�C5 as given in
Table 6.1. The definition of symbols for the cellular steel beams modeled
by Ellobody [6.17] is shown in Figure 6.7. Specimen C1, tested in Ref.
[6.33], had a length (L) of 5.25 m and was fabricated from hot-rolled
I-section UB 4063 1403 39. The top and bottom flanges of C1 were
braced laterally every 1 m as shown in Figure 6.8. The cellular steel beam
D
L/2L1
h=H–t
Lateral bracing positions
B
Roller support
position
L2
Applied load
Figure 6.7 Definition of symbols and finite element mesh for the cellular steel beam
C2 [6.17,6.34].
135Examples of Finite Element Models of Metal Beams
C1 was loaded with two concentrated loads, with a spacing from the
support (L1) as given in Table 6.1. The beam had a cell diameter (D) of
375 mm and a depth (H) of 581 mm, with D/H ratio of 0.65. The spac-
ing between the centerlines of two adjacent circular cells (L2) was
Applied load
Lateral bracing positions
Roller support
position(A)
(B)
(C)
Symmetry surface
Applied load
Roller support
position Applied load
Symmetry
surface
Roller support position
Figure 6.8 Finite element meshes for cellular steel beams modelled investigated
[6.17,6.33�6.36]. (A) Specimen C1 tested in Ref. [6.33]. (B) Specimen C3 tested in Ref.
[6.35]. (C) Specimens C4 and C5 tested in Ref. [6.36].
136 Finite Element Analysis and Design of Metal Structures
461 mm, with L2/D ratio of 1.23. The main failure mode observed
experimentally for C1 was interaction of WDB and WPB failure modes
(WDB1WPB). The cellular steel beam test specimen C2, tested in Ref.
[6.34], had a length (L) of 7.4 m and was fabricated from hot-rolled
I-section UB 3053 1023 25. The top and bottom flanges of C2 were
braced laterally as shown in Figure 6.7. The cellular steel beam C2 was
loaded with two concentrated loads. The cell diameter and depth of the
beam were 325 and 463.2 mm, respectively, with D/H ratio of 0.7. The
spacing between the centerlines of two adjacent circular cells was
400 mm, with L2/D ratio of 1.23. Similar to C1, the main failure mode
observed experimentally for C2 was interaction of WDB and WPB fail-
ure modes (WDB1WPB).
The cellular steel beam test C3, detailed in Ref. [6.35], had a length
(L) of 1.5 m and was fabricated from hot-rolled I-section UB
3053 1653 40. The main purpose of the test was to investigate the shear
resistance of cellular steel beams. The steel grade was S275. The cellular
steel beam C3 was braced laterally as shown in Figure 6.8. The cell diam-
eter and depth of the beam were 231 and 303.4 mm, respectively, with
D/H ratio of 0.76. The cellular steel beam C3 had only two circular cells
with spacing between the centerlines of the two cells given in Table 6.1.
The main failure mode observed experimentally for C3 was interaction
of LWB and SY failure modes (LWB1 SY). Finally, the cellular steel
beams C4 and C5, tested in Ref. [6.36], had a length (L) of 1.7 m and
was fabricated from hot-rolled I-section UB 4573 1523 52. The steel
grade was S355. The main variable parameter in the tests was the spacing
between the web cells. The cellular steel beams C4 and C5 were braced
laterally as shown in Figure 6.8. The circular cell diameter and depth of
Table 6.1. Dimensions and Material Properties of Cellular Steel Beams Modeled in
Ref. [6.17]
Test
Dimensions (mm)
Material
Properties
fy (MPa)
Ref-
erencesH B t s L L1 L2 h D Flange Web
C1 581.0 141.8 8.6 6.4 5250 1575 461.0 572.4 375 401.0 392.0 [6.33]
C2 463.2 101.6 7.0 5.8 7400 2466 400.0 452.5 325 401.0 392.0 [6.34]
C3 303.4 165.0 10.2 6.0 1500 600 900.0 293.2 231 337.5 299.0 [6.35]
C4 449.8 152.4 10.9 7.6 1700 850 409.5 438.9 315 359.6 375.3 [6.36]
C5 449.8 152.4 10.9 7.6 1700 850 378.0 438.9 315 359.6 375.3 [6.36]
137Examples of Finite Element Models of Metal Beams
the beams were 315 and 449.8 mm, respectively, with D/H ratio of 0.7.
The spacing between the centerlines of two adjacent circular cells were
409.5 and 378 mm, with L2/D ratios of 1.3 and 1.2, respectively, for
beams C4 and C5. Similar to C3, the main failure mode observed experi-
mentally for C4 and C5 was interaction of LWB and SY failure modes
(LWB1 SY). Further details regarding the destructive full-scale cellular
steel beam tests investigated in this study are given in Refs [6.33�6.36].
The test program provided useful and detailed data regarding the behavior
of castellated steel beams. Therefore, finite element analysis was per-
formed on the castellated steel beams.
The finite element program ABAQUS [1.27] was used in the analysis
of cellular steel beams with circular holes tested by Surtees and Liu
[6.33], Warren [6.34], Tsavdaridis and D’Mello [6.35], and Tsavdaridis
et al. [6.36]. The models, developed by Ellobody [6.17], accounted for
the measured geometry, initial geometric imperfections, and measured
material properties of flange and web portions. A combination of 4-node
and 3-node doubly curved shell elements with reduced integration S4R
and S3R, respectively, were used to model the flanges and web of the
cellular steel beams, as shown in Figures 6.7 and 6.8. Since lateral
buckling of cellular steel beams is very sensitive to large strains, the S4R
and S3R elements were used in this study to ensure the accuracy of the
results. In order to choose the finite element mesh that provides accurate
results with minimum computational time, convergence studies were
conducted. It was found that approximately 403 50 mm (length by width
of S4R element and depth by width of S3R element) ratio provides ade-
quate accuracy in modeling the web while a mesh of approximately
353 50 mm was used in the flange.
The finite element analysis investigated in this study accounts for both
geometrical and material nonlinearities. Hence, the application of bound-
ary conditions is very important. Only half of the beams was modeled
where there is exact symmetry in loading, geometry, and boundary con-
ditions (see Section 3.3). The results obtained from modeling half of the
beam has to be first compared with that obtained from modeling of the
full beams and calibrated against the test results. In this study, it was found
that modeling half of the beams C1, C2, C4, and C5 provide accurate
results when verified against the test results while beam C3 was modeled
in full as shown in Figures 6.7 and 6.8. Since the lateral bracing system
used in the tests [6.33�6.36] was quite rigid preventing lateral transitional
displacement and allowing rotational displacements, the top compression
138 Finite Element Analysis and Design of Metal Structures
flange was prevented from lateral transitional displacement at the positions
detailed in the tests. The load was applied in increments as static point
load using the Riks method available in the ABAQUS [1.27] library. The
stress�strain curve for the structural steel given in the EC3 [6.24] was
adopted in Ref. [6.17] with measured values of the yield stress (fy) and
ultimate stress (fu) used in the tests [6.33�6.36]. The material behavior
provided by ABAQUS [1.27] (using the PLASTIC option) allows a non-
linear stress�strain curve to be used (see Section 3.4).
Buckling of cellular beams depends on the lateral restraint conditions
to compression flange and geometry of the beams. The lateral distortional
buckling modes could be obtained by performing eigenvalue buckling
analysis for cellular beams with actual geometry and actual lateral restraint
conditions to the compression flange. Figures 6.9 and 6.10 show examples
of unrestrained between ends and restrained bucklingmodes along the
compression flange of cellular steel beams, respectively. Only the first
buckling mode (eigenmode 1) is used in the eigenvalue analysis. Since
buckling modes predicted by ABAQUS eigenvalue analysis [1.27] are
generalized to 1.0, the buckling modes are factored by a magnitude of
Lu/1000, where Lu is the length between points of effective bracing. The
factored buckling mode is inserted into the load�displacement nonlinear
analysis of the cellular beams following the eigenvalue prediction. It
should be noted that the investigation of cellular steel beams with differ-
ent slenderness ratios could result in LTB mode with or without WDB
Deformed shape
Undeformed shape
Symmetry surface
Roller support
Figure 6.9 Unrestrained elastic lateral distortional buckling mode (eigenmode 1) for
the cellular steel beam specimen C2 [6.17,6.34].
139Examples of Finite Element Models of Metal Beams
and WPB modes. Hence, to ensure that the correct buckling mode is
incorporated in the nonlinear displacement analysis, the eigenvalue buck-
ling analysis must be performed for each cellular steel beam with actual
geometry. More details regarding modeling of geometric imperfections
can be found in Section 4.3. The cellular steel beams investigated in this
study were fabricated by cutting a solid web of hot-rolled doubly sym-
metric I-section and reassembling it by shifting and welding the section
components. Assuming that the cutting process is carefully conducted,
the distribution of residual stresses within the cellular beam can be simu-
lated as that of doubly symmetric I-sections. A typical distribution of
residual stresses in hot-rolled doubly symmetric I-sections recommended
in Ref. [6.37] was used in Ref. [6.17]. The residual stresses are imple-
mented in the finite element model as initial stresses before applying
loads. This can be performed using the (�INITIAL CONDITIONS,
TYPE5 STRESS) parameter available in the ABAQUS [1.27] library.
Detailed information regarding modeling residual stresses can be found in
Section 3.6.
The cellular steel beam tests detailed in Refs [6.33�6.36] were mod-
eled by Ellobody [6.17]. The beams had different cross section geome-
tries, lengths, steel strengths, and failure modes, which ensure that the
model is capable to predict the inelastic behavior of a wide range of cellu-
lar steel beams. The failure loads, mid-span deflection at failure, failure
modes, and load�mid-span deflection curves observed experimentally
were compared with that predicted numerically using the finite element
model. Table 6.2 gives a comparison between the failure loads (PTest) and
mid-span deflections at failure (δTest) obtained from the tests and finite
element analyses (PFE) and (δFE), respectively. It can be seen that good
Symmetry surface
Undeformed shape
Deformed shape
Roller support
Figure 6.10 Restrained elastic lateral distortional buckling and WPB mode (eigen-
mode 1) for the cellular steel beam specimen C5 [6.17,6.34].
140 Finite Element Analysis and Design of Metal Structures
agreement was achieved between the test and finite element results. The
mean value of PTest/PFE and δTest/δFE ratios are 0.99 and 0.96, respec-
tively, with the COV of 0.02 and 0.08, respectively, as given in Table 6.2.
Four failure modes were observed experimentally and confirmed numeri-
cally using the finite element model as summarized in Table 6.2. The cel-
lular steel beams tested in Refs [6.33,6.34] underwent WDB that
followed by WPB. The cellular steel beam tested in Ref. [6.35], having a
length of 1.5 m, underwent LWB followed by SY. The SY failure mode
was predicted from the finite element model by comparing the von Mises
stresses in the cellular steel beams at failure against the measured yield
stresses. On the other hand, the SY was judged in the tests by comparing
the test failure loads against the plastic collapse loads (Ppx) calculated
according to AS4100 [6.16]. Finally, the cellular steel beams tested in
Ref. [6.36], having a length of 1.7 m, underwent WPB followed by SY.
The load�mid-span deflection curves predicted experimentally and
numerically were also compared as shown in Figures 6.11 and 6.12 as
examples for beam tests C1 and C2. It can be shown that generally good
agreement was achieved between experimental and numerical
relationships.
Furthermore, the deformed shapes of cellular steel beams at failure
observed experimentally and numerically were compared. Figure 6.13
shows an example of the displaced shape observed in the test specimen C3
in comparison with that predicted from the finite element analysis. It can
be seen that the experimental and numerical deformed shapes are in good
agreement. The failure mode observed experimentally and confirmed
numerically was a combination of LWB and SY. The data obtained from
Table 6.2 Comparison of Test and Finite Element Results of Cellular Steel Beams
[6.17]
Test
[Reference]
Test Finite Element Analysis
PTest
(kN)
δTest
(mm)
Failure
Mode
PFE
(kN)
δFE
(mm)
Failure
Mode PTest
PFE
δTest
δFE
C1 [33] 188.5 17.3 WDB1WPB 193.7 19.7 WDB1WPB 0.97 0.88
C2 [34] 114.0 48.0 WDB1WPB 113.0 51.2 WDB1WPB 1.01 0.94
C3 [35] 274.6 22.0 LWB1 SY 281.9 20.3 LWB1 SY 0.98 1.06
C4 [36] 288.7 19.6 WPB1 SY 287.0 20.5 WPB1 SY 1.01 0.96
C5 [36] 255.0 26.0 WPB1 SY 263.9 28.0 WPB1 SY 0.97 0.93
Mean � � � � � � 0.99 0.96
COV � � � � � � 0.020 0.080
141Examples of Finite Element Models of Metal Beams
0
80
40
120
160
200
240
0 10 20 30 40 6050
Mid-span deflection (mm)
Lo
ad
 (
kN
)
Test
FE
Figure 6.11 Comparison of load�mid-span deflection curves for test specimen C1.
0
40
20
60
80
100
120
140
0 20 40 60 80 100
Mid-span deflection (mm)
Lo
ad
 (
kN
)
Test
FE
Figure 6.12 Comparison of load�mid-span deflection curves for test specimen C2.
(A)
Support stiffener
(B)
Local web
buckling
Steel flange yielding 
Steel flange
yielding
Local web
buckling
Figure 6.13 Comparison of experimental (B) and numerical (A) buckled shapes at
failure for Specimen C3 [6.17,6.35].
142 Finite Element Analysis and Design of Metal Structures
ABAQUS [1.27] have shown that the von Mises stresses at the maximum
stressed fibers at the top and bottom flanges under the applied load
exceeded the measured yield stresses. Similarly, Figure 6.14 shows another
example of the displaced shape observed in the test specimen C4 in com-
parison with that predicted from the finite element analysis. Once again, it
can be seen that good agreement exists between the experimental and
numerical deformed shapes. The failure mode observed experimentally and
confirmed numerically was a combination of WPB and SY.
The verified finite element model developed in Ref. [6.17] was used
to study the effects of the change in cross section geometries, beam
length, steel strength, and nondimensional slenderness on the strength
and buckling behavior of cellular steel beams. One hundred and twenty
cellular steel beams were analyzed using the finite element model. The
beams were divided into 12 groups denoted G1�G12. The first six
groups G1�G6 had beams with a length of (L) 5250 mm and a depth
(H) of 581 mm, while groups G7�G12 had beams with a length of
7400 mm and a depth of 463.2 mm, which is similar to the beam
lengths of test specimens C1 and C2, respectively. The cellular steel
beams in G1�G6 had a cell diameter (D) of 325 mm and spacing
between centerlines of two adjacent cells (L2) of 525 mm, with (D/H)
and (L2/D) ratios of 0.56 and 1.62, respectively. On the other hand, the
cellular steel beams in G7�G12 had the same D of 325 mm and L2 of
400 mm, with (D/H) and (L2/D) ratios of 0.7 and 1.23, respectively.
Group G1 had 10 cellular steel beams S1�S10 having a height (h) of
572.4, a width (B) of 141.8 mm, and a web thickness (s) of 6.4 mm, but
with different flange thickness (t) ranging from 4 to 16 mm. This has
(A) (B)
Mid-symmetry surface 
Web-post buckling
Support stiffenerFigure 6.14 Comparison of experimental (B) and numerical (A) buckled shapes at
failure for Specimen C4 [6.17,6.36].
143Examples of Finite Element Models of Metal Beams
resulted in B/t ratios ranging from 35.5 to 8.9. Group G1 had a steel
yield stress (fy) of 275 MPa and an ultimate stress (fu) of 430 MPa.
Groups G2 and G3 were identical to G1 except with fy of 460, and
690 MPa and fu of 530 and 760 MPa, respectively. The yield and ulti-
mate stresses conform to EC3 [6.24]. Group G4 had 10 specimens
S31�S40 having h of 572.4, B of 141.8 mm, and t of 8.6 mm but with
different s ranging from 4 to16 mm. This has resulted in h/s ratios vary-
ing from 143.1 to 35.8. Groups G5 and G6 were identical to G4 but
with different steel yield and ultimate stresses. Groups G4�G6 had the
same steel stresses as G1�G3, respectively.
Group G7 had 10 cellular steel beams S61�S70 having h of 452.5, B of
123.3 mm, and s of 7.1 mm, but with different t ranging from 4 to 16 mm.
This has resulted in B/t ratios ranging from 30.8 to 7.7. Group G7 had a
steel yield stress (fy) of 275 and an ultimate stress (fu) of 430 MPa. Groups G8
and G9 were identical to G7 except with fy of 460 and 690 MPa and fu of
530 and 760 MPa, respectively. Group G10 had 10 specimens S91�S100
having h of 452.5, B of 123.3 mm, and t of 10.7 mm but with different s
ranging from 4 to16 mm. This has resulted in h/s ratios varying from 113.1
to 28.3. Groups G11 and G12 were identical to G4 but with different steel
yield and ultimate stresses. Groups G10�G12 had the same steel stresses as
G7�G9, respectively. The investigated cellular steel beams had different
nondimensional slenderness (λ) calculated based on AS4100 [6.16] ranged
from 0.66 to 1.93. The nondimensional slenderness (λ) is equal to the square
root of the major axis full plastic moment divided by the elastic buckling
moment, and is considered as a guide for beam slenderness in this study.
To date, there is no design guides in current codes of practice that
account for the inelastic behavior of normal and high strength cellular steel
beams under combined buckling modes including WDB. Only design
guides were found in the AS4100 [6.16] that considers LTB of doubly sym-
metric I-sections as well as design guides in the AISC [6.38] that controls the
errors associated with neglecting web distortion in doubly symmetric
I-sections. Zirakian and Showkati [6.27] have concluded that the AISC
[6.38] predictions are overconservative and in some cases may cause eco-
nomic losses for doubly symmetric I-sections under distortional buckling. In
the study [6.17], the failure loads of the cellular steel beams investigated in
the parametric study were compared with the design guides given in the
AS4100 [6.16]. Following the AS4100 design guides [6.16], the nominal
buckling moment strength (Mb) of compact doubly symmetric I-section
beams is given by
144 Finite Element Analysis and Design of Metal Structures
Mb 5αmαsMpx ð6:1Þ
where Mpx5 fySx is the major axis full plastic moment corresponding to
collapse load Ppx, fy is the yield stress, Sx is the plastic section modulus, αm
is a moment modification factor which allows for nonuniform moment
distributions (taken 1.0 for simply supported beams under two concen-
trated loads), and αs is a slenderness reduction factor which allows for the
effects of elastic buckling, initial geometric imperfections, initial twist, and
residual stresses, and which is given by Trahair [6.39] as follows:
αs5 0:6
ffiffiffiffiffiffiffiffiffiffiffiffiffiffiffiffiffiffiffiffiffiffiffiffi
Mpx
Myz
	 
2
1 3
s
2
Mpx
Myz
	 
0
@
1
A# 1:0 ð6:2Þ
where Myz is the elastic buckling moment of a simply supported beam in
uniform bending given by
Myz5
ffiffiffiffiffiffiffiffiffiffiffiffiffiffiffiffiffiffiffiffiffiffiffiffiffiffiffiffiffiffiffiffiffiffiffiffiffiffiffiffiffiffiffi
π2EIy
Lu
2
GJ1
π2EIw
Lu
2
	 
s
ð6:3Þ
where E and G are the Young’s modulus and shear modulus of elasticity,
Iy, J and Iw are the minor axis section moment of area, the uniform tor-
sion section constant, and the warping section constant, respectively. The
nondimensional slenderness (λ) of the cellular steel beam according to
AS4100 is equal to
ffiffiffiffiffiffiffiffiffiffiffiffiffiffiffiffiffiffi
Mpx=Myz
p
and is considered as a guide for beam
slenderness in this study. The design load of cellular steel beams, with
simply supported ends under two concentrated loads, based on AS4100
(PAS4100) is calculated from Mb.
Figure 6.15 plots the failure loads of cellular steel beams in groups
G1�G3 predicted from the finite element analysis (PFE) and design guides
(PAS4100). The failure loads were plotted, as a percentage of the plastic
collapse load (Ppx), against the nondimensional flange width-to-thickness
ratio (B/t). Looking at the cellular steel beams in G1, it can be seen that
as the B/t ratio increased from 8.9 to 20.3, the PFE/Ppx ratio is increased
nonlinearly. While increasing the B/t ratio above 20.3 has resulted in
approximately nonlinear decrease in the PFE/Ppx ratio. However, interest-
ingly, as the B/t ratio increased from 8.9 to 35.5, the PAS4100/Ppx ratio is
reduced in a nonlinear relationship. This is attributed to the fact that for
cellular steel beams having less B/t, the failure mode was dominated by
the presence of combined (WDB1WPB), which was not considered by
the specification [6.16]. The comparison has also shown that the AS4100
145Examples of Finite Element Models of Metal Beams
design guides are generally conservative for the cellular steel beams with
normal yield strength (beams in G1), except for beams S9 and S10 failing
by (LTB1WDB1WPB). Similar conclusions were observed for beams
in G2 and G3 having higher steel strengths with fy of 460 and 690 MPa,
respectively, as shown in Figure 6.15. However, it can be seen that the
specification predictions were quite conservative for the beams with high-
er yield stresses (beams in G2 and G3) and failing by LTB. Similar
0.00
0.20
0.40
0.60
0.80
1.00
0 4 8 12 16 20 24 28 32 4036
B/t
P
F
E
/P
px
 a
nd
 P
A
S
41
00
/P
px
FE (G1)
AS4100 (G2)
FE (G3)
AS4100 (G3)
AS4100 (G1)
FE (G2)
Figure 6.15 Comparison of finite element analysis and design predictions for cellular
steel beams in groups G1�G3 [6.17].
0.00
0.20
0.40
0.60
0.80
1.00
0 4 8 12 16 20 24 28 32 4036
B/t
P
F
E
/P
px
 a
nd
 P
A
S
41
00
/P
px
FE (G7)
AS4100 (G8)
FE (G9)
AS4100 (G9)
AS4100 (G7)
FE (G8)
Figure 6.16 Comparison of finite element analysis and design predictions for cellular
steel beams in groups G7�G9 [6.17].
146 Finite Element Analysis and Design of Metal Structures
conclusions could be drawn for the cellular steel beams in G7�G9 as
shown in Figure 6.16.
Figures 6.17 and 6.18 plots the PFE/Ppx and PAS4100/Ppx ratios against
the nondimensional web height-to-web thickness ratio (h/s) for the cellu-
lar steel beams in G4�G6 and G10�G12. Looking at Figure 6.17, it can
be seen that there is a dramatic decrease in the failure load of cellular steel
beams having h/s ratios greater than or equal to 104.1 and failing mainly
0.00
0.20
0.40
0.60
0.80
1.00
0 20 40 60 80 100 120 160140
h/s
P
F
E
/P
px
 a
nd
 P
A
S
41
00
/P
px
FE (G4) AS4100 (G6)
AS4100 (G5) AS4100 (G4)
FE (G6) FE (G5)
Figure 6.17 Comparison of finite element analysis and design predictions for cellular
steel beams in groups G4�G6 [6.17].
0.00
0.20
0.40
0.60
0.80
1.00
0 20 40 60 80 100 120 140
h/s
P
F
E
/P
px
 a
nd
 P
A
S
41
00
/P
px
FE (G10) AS4100 (G12)
AS4100 (G11) AS4100 (G10)
FE (G12) FE (G11)
Figure 6.18 Comparison of finite element analysis and design predictions for cellular
steel beams in groups G10�G12 [6.17].
147Examples of Finite Element Models of Metal Beams
owing to the combined WDB and WPB failure mode. It can also be seen
that some cellular steel beams with fy of 275 MPa failed due to plastic col-
lapse, while none of the cellular steel beams withfy of 460 and 690 MPa
exceeded the plastic resistance. The specification predictions were uncon-
servative for the cellular steel beams undergoing combined WDB and
WPB failure mode. The specification predictions were generally conser-
vative for cellular steel beams with normal yield strength and failing
mainly by LTB. However, the specification predictions were quite conser-
vative for cellular steel beams with higher yield stresses and once again
failing mainly by LTB. Similar conclusions could be drawn for the cellular
steel beams in G10�G12 as shown in Figure 6.18.
REFERENCES
[6.1] Liu, T. C. H. and Chung, K. F. Steel beams with large web openings of various
shapes and sizes: Finite element investigation. Journal of Constructional Steel
Research, 59(9), 1159�1176, 2003.
[6.2] Chung, K. F., Liu, T. C. H. and Ko, A. C. H. Investigation on Vierendeel mecha-
nism in steel beams with circular web openings. Journal of Constructional Steel
Research, 57(5), 467�490, 2001.
[6.3] Redwood, R. G. and McCutcheon, J. O. Beam tests with un-reinforced web
openings. Journal of Structural Division, Proceedings of ASCE, 94(ST1), 1�17,
1968.
[6.4] Mohri, F., Brouki, A. and Roth, J. C. Theoretical and numerical stability analyses
of unrestrained, mono-symmetric thin-walled beams. Journal of Constructional
Steel Research, 59(1), 63�90, 2003.
[6.5] Zhu, J. H. and Young, B. Design of aluminum alloy flexural members using direct
strength method. Journal of Structural Engineering, ASCE, 135(5), 558�566,
2009.
[6.6] Liu, Y. and Gannon, L. Finite element study of steel beams reinforced while under
load. Engineering Structures, 31(11), 2630�2642, 2009.
[6.7] Gannon, L. Strength and behavior of beams strengthened while under load. MSc
thesis. Halifax (NS, Canada): Department of Civil and Resource Engineering,
Dalhousie University; 2007.
[6.8] Wu, Z. Q. and Grondin, G. Y. Behavior of steel columns reinforced with welded
steel plates. Structural Engineering Report no. 250. Edmonton (AB, Canada):
Department of Civil and Environmental Engineering, University of Albert; 2002.
[6.9] Theofanous, M. and Gardner, L. Experimental and numerical studies of lean
duplex stainless steel beams. Journal of Constructional Steel Research, 66(6),
816�825, 2010.
[6.10] Theofanous, M., Chan, T. M. and Gardner, L. Structural response of stainless steel
oval hollow section compression members. Engineering Structures, 31(4),
922�934, 2009.
[6.11] Theofanous, M., Chan, T. M. and Gardner, L. Flexural behaviour of stainless steel
oval hollow sections. Thin-Walled Structures, 47(6�7), 776�787, 2009.
[6.12] Sweedan, A. M. I. Elastic lateral stability of I-shaped cellular steel beams. Journal
of Constructional Steel Research, 67(2), 151�163, 2011.
148 Finite Element Analysis and Design of Metal Structures
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref1
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref1
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref1
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref1
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref2
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref2
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref2
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref2
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref3
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref3
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref3
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref3
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref4
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref4
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref4
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref4
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref5
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref5
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref5
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref5
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref6
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref6
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref6
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref7
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref7
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref7
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref7
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref8
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref8
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref8
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref8
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref9
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref9
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref9
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref9
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref10
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref10
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref10
[6.13] Haidarali, M. R. and Nethercot, D. A. Finite element modelling of cold-formed
steel beams under local buckling or combined local/distortional buckling. Thin-
Walled Structures, 49(12), 1554�1562, 2011.
[6.14] CUFSM Version 3.12, by Ben Schafer. Department of Civil Engineering, Johns
Hopkins University; 2006.
[6.15] Ellobody, E. Interaction of buckling modes in castellated steel beams. Journal of
Constructional Steel Research, 67(5), 814�825, 2011.
[6.16] Australian Standards AS4100. Steel Structures. AS4100-1998. Sydney, Australia:
Standards Australia, 1998.
[6.17] Ellobody, E. Nonlinear analysis of cellular steel beams under combined buckling
modes. Thin-Walled Structures, 52(3), 66�79, 2012.
[6.18] Anapayan, T. and Mahendran, M. Numerical modelling and design of LiteSteel
Beams subject to lateral buckling. Journal of Constructional Steel Research, 70,
51�64, 2012.
[6.19] Kurniawan, C. W. and Mahendran, M. Elastic lateral buckling of simply supported
LiteSteel Beams subject to transverse loading. Thin-Walled Structures, 47(1),
109�119, 2009.
[6.20] Zhou, F., Young, B. and Lam, H. C. Welded aluminum alloy plate girders sub-
jected to shear force. Advanced Steel Construction, 8(1), 71�94, 2012.
[6.21] Soltani, M. R., Bouchaı̈r, A. and Mimoune, M. Nonlinear FE analysis of the ulti-
mate behavior of steel castellated beams. Journal of Constructional Steel Research,
70, 101�114, 2012.
[6.22] Lusas 13. LUSAS: finite element stress analysis system: user’s manual. Finite
Element Analysis Ltd. Version 13.5, UK, 2003.
[6.23] Kankanamge, N. D. and Mahendran, M. Behaviour and design of cold-formed
steel beams subject to lateral-torsional buckling. Thin-Walled Structures, 51,
25�38, 2012.
[6.24] European Committee for Standardization (ECS), Eurocode 3. Design of steel
structures—Part 1.3, general rules—supplementary rules for cold-formed thin
gauge members and sheathing. Brussels: Eurocode 3, 2006.
[6.25] Standards Australia/New Zealand. Cold-formed steel structures. AS/NZS 4600.
Sydney, Australia: 2005.
[6.26] American Iron and Steel Institute (AISI). North American specification for the
design of cold-formed steel structural members. Washington DC: American Iron
and Steel Institute, 2007.
[6.27] Zirakian, T. and Showkati, H. Distortional buckling of castellated beams. Journal
of Constructional Steel Research, 62(9), 863�871, 2006.
[6.28] Bradford, M. A. Lateral-distortional buckling of steel I-section members. Journal
of Constructional Steel Research, 23(1-3), 97�116, 1992.
[6.29] Nethercot, D. A. and Trahair, N. S. Inelastic lateral buckling of determinate
beams. Journal of Structural Division, ASCE, 102(ST4), 701�717, 1976.
[6.30] Zhu, J. H. and Young, B. Experimental investigation of aluminum alloy thin-
walled tubular members in combined compression and bending. Journal of
Structural Engineering, ASCE, 132(12), 1955�1966, 2006.
[6.31]Schafer, B. W. and Peköz, T. Direct strength prediction of cold-formed steel mem-
bers using numerical elastic buckling solutions. Proceedings of 14th International
Specialty Conference on Cold-Formed Steel Structures, University of Missouri-
Rolla, Rolla, MO; 69�76, 1998.
[6.32] Zhu, J. H. and Young, B. Aluminum alloy tubular columns—Part II: Parametric
study and design using direct strength method. Thin-Walled Structures, 44(9),
969�985, 2006.
149Examples of Finite Element Models of Metal Beams
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref11
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref11
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref11
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref11
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref12
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref12
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref12
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref13
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref13
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref14
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref14
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref14
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref15
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref15
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref15
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref15
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref16
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref16
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref16
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref16
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref17
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref17
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref17
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref18
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref18
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref18
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref18
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref19
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref19
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref19
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref19
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref20
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref20
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref20
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref21
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref21
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref22
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref22
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref22
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref23
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref23
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref23
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref24
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref24
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref24
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref25
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref25
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref25
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref26
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref26
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref26
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref26
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref27
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref27
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref27
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref27
[6.33] Surtees, J. O. and Liu, Z. Report of loading tests on cellform beams. Research
report, University of Leeds; 1995.
[6.34] Warren, J. Ultimate load and deflection behaviour of cellular beams. MSc thesis.
Durban: School of Civil Engineering, University of Natal; 2001.
[6.35] Tsavdaridis, K. D. and D’Mello, C. Web buckling study of the behaviour and
strength of perforated steel beams with different novel web opening shapes.
Journal of Constructional Steel Research, 67, 1605�1620, 2011.
[6.36] Tsavdaridis, K. D., D’Mello, C., and Hawes, M. Experimental study of ultra shal-
low floor beams with perforated steel sections. Research report, National Specialist
Contractors’ Council, NSCC2009; 312�319, 2009.
[6.37] Chen, S. and Jia, Y. Numerical investigation of inelastic buckling of steel-concrete com-
posite beams prestressed with external tendons. Thin-Walled Structures, 48, 233�242,
2010.
[6.38] AISC. Specification for structural steel buildings. American Institute for Steel
Construction, Reston, Chicago, IL, ANSI/AISC 360-05 2005.
[6.39] Trahair, N. S. Flexural-torsional buckling of structures. London: E & FN Spon,
1993.
150 Finite Element Analysis and Design of Metal Structures
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref28
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref28
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref28
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref28
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref29
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref29
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref29
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref29
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref30
http://refhub.elsevier.com/B978-0-12-416561-8.00006-8/sbref30
CHAPTER77
Examples of Finite Element
Models of Metal Tubular
Connections
7.1. GENERAL REMARKS
The finite element modeling of metal columns and beams have been
highlighted in Chapters 5 and 6, respectively, and examples of finite ele-
ment models of metal connections are presented in this chapter. The con-
nections investigated in this book can be constructed from any metal
material. The connections investigated can be different boundary condi-
tions at the ends and can be rigid or semi-rigid connections. In addition,
the connections investigated can have different cross sections constructed
from hot-rolled, cold-formed, and welded sections. It should be noted
that there are many types of connections that are used in practice, which
may need a separate book to provide full details. However, this book pro-
vides an approach for modeling metal connections which can be applied
to different types of connections. Therefore, based on recent investiga-
tions by the authors, it is decided to present an innovative type of metal
connections which are cold-formed stainless steel tubular joints. Cold-
formed stainless steel tubular joints are being used increasingly for archi-
tectural and structural purposes due to their aesthetic appearance, high
corrosion resistance, ductility property, improved fire resistance, and ease
of construction and maintenance. The practical applications of cold-
formed welded tubular joints are shown in Figures 7.1�7.3. To date,
there is little research being carried out on cold-formed stainless steel
tubular joints. Furthermore, the current design rules for stainless steel
tubular joints are mainly based on the carbon steel sections. The mechan-
ical properties of stainless steel sections are clearly different from those of
carbon steel sections. Stainless steel sections have a rounded stress�strain
curve with no yield plateau and low proportional limit stress compared to
carbon steel sections, as shown in Figure 1.1. To facilitate the use of stain-
less steel tubular structures, design guidelines should be prepared for
151
Finite Element Analysis and Design of Metal Structures
DOI: http://dx.doi.org/10.1016/B978-0-12-416561-8.00007-X
© 2014 Elsevier Inc.All rights reserved.
http://dx.doi.org/10.1016/B978-0-12-416561-8.00007-X
stainless steel tubular hollow sections to offset its high material costs
through efficient design.
Numerical investigations on cold-formed stainless steel tubular
T-joints, X-joints, and X-joints with chord preload are current research
Figure 7.1 Curtain wall construction of Langham Place in Hong Kong, China.
Figure 7.2 Roof structure of Kuala Lumpur International Airport, Malaysia.
152 Finite Element Analysis and Design of Metal Structures
topics. The stainless steel tubular joints, highlighted in this book, were
fabricated from square and rectangular hollow sections (SHS and RHS)
brace and chord members. A test program carried out on a wide range of
cold-formed stainless steel tubular T- and X-joints of SHS and RHS is
introduced in this chapter. The corresponding finite element models
developed based on the experimental investigations are described in
detail. This chapter highlights how the geometric and material nonlinea-
rities of stainless steel tubular joints can be carefully incorporated in the
finite element models. This chapter also presents the results obtained from
experimental investigations and finite element analyses comprising the
joint strengths, failure modes, and load�deformation curves of stainless
steel tubular joints.
This chapter initially presents a survey of recent published numerical,
using finite element method, investigations on metal connections. After
that, the chapter presents the experimental investigations and finite
element models previously published by the authors for different metal
tubular connections. The joint strengths, failure modes, and
load�deformation curves of cold-formed stainless steel tubular T-
and X-joints obtained experimentally and numerically are highlighted
and discussed to show the effectiveness of the results. In addition, this
Figure 7.3 Footbridge in Singapore.
153Examples of Finite Element Models of Metal Tubular Connections
chapter presents the comparison between the experimental and finite ele-
ment analysis results to calibrate the developed finite element models.
The authors highlight how the information presented in the previous
chapters is used to develop the examples of finite element models to
accurately simulate the structural behavior of test specimens introduced in
this chapter. The authors have an aim that the examples highlighted in
this chapter can explain to readers the effectiveness of finite element mod-
els in providing detailed data that augment experimental investigations
conducted in the field. The results are discussed to show the significance
of the finite element models in predicting the structural response of dif-
ferent metal structural connections. The authors also have an aim that by
highlighting the structural performance of metal tubular connections,
researchers can use the same approach to investigate the building struc-
tural behavior.
7.2. PREVIOUS WORK
Finite element analysis can be used effectively to highlight the perfor-
mance of metal connections, with many different general-purpose finite
element analysis software can be used such as ANSYS [5.3], ABAQUS
[1.27], I-DEAS [7.1], MARC [7.2], PAFEC [7.3], and PATRAN [7.4].
Finite element analysis can be used to investigate the behavior of cold-
formed welded circular hollow section (CHS), SHS, and RHS tubular
joints, which are discussed in this chapter. The accuracy of finite element
analysis of metal connections mainly depends on the use of proper finite
element type, material modeling, analysis procedure, integration scheme,
loading and boundary condition, mesh refinement, and modeling of weld
shape, as presented in the previous chapters.
Extensive investigations were presented in the literature detailing the
performance of metal connections through using the finite element analy-
sis. Packer [7.5] undertook a parametric study to identify the principal
factors that affect the behavior and ultimate strength of statically loaded
welded joints in RHS steel trusses, having one compression bracing
member and one tension bracing member. The numerical investigation
was validated by comparing with a large number of test results, which
mainly examined cases in which the bracing members are gapped as well
as overlapped at the chord face connection. The influential factors investi-
gated in the parametric study include the yield stress, chord force, strut
dimensions relative to the chord in overlapped joints, amount of gap or
154 Finite Element Analysis and Design of Metal Structures
overlap, orientation of bracing members in gapped joints, and width ratio
between bracing members and chord in gapped joints and the bracing
member angles. Simplified design formulae were also proposed to predict
the ultimate joint strength.
Packer et al. [7.6] described a finite element model for a welded
gapped K-joint in a RHS warren truss to study the parameters
influencing the flexibility of joint at the serviceability limit state.
A bilinear elastic-strain hardening material characteristic was incorporated
and large deflection behavior of both the chord face and the supporting
frames was included in the model. It was found that optimum correlation
between chord face deformations is primarily dependent on the stress
distribution assumed around the perimeter of the branch members at the
chord face junction, with the flexibility of the inclusions beneath the
branch members also being influential. Ebecken et al. [7.7] established
nonlinear elasto-plastic finite element models to determine the static
strength of typical X-joint under axial brace loads. Techniques for auto-
matically generating finite element meshes in stress analysis of tubular
intersections were used. Only one-eighth of the tubular joint was
modeled due to the symmetric loading and boundary conditions. The
results were obtained by using 3-node flat shell element and 8-node iso-
parametric shell element. The modeling and computational aspects which
are required for dealing with the elasto-plastic analysis were discussed to
obtain the ultimate joint strengths.
Zhang et al. [7.8] developed a suitable nonlinear finite element model
that incorporated large deflection to conduct elasto-plastic analysis of the
ultimate strength of welded RHS joints. The comparison between
experimental and numerical results showed good agreement. A model
called the equivalent frame tube model which can properly simulate the
characteristic of the ultimate strength of RHS joints was proposed.
A design formula was derived to predict the ultimate strength of RHS
X-joints. Moffat et al. [7.9] carried out nonlinear finite element analysis
to assess the static collapse strength of a sample tubular T-joint configura-
tion subjected to compressive brace loading. Two series of models were
used to assess the effects of varying the chord length and chord boundary
conditions on the ultimate joint strengths. The finite element model was
produced using the PATRAN [7.4] mesh generation program. The static
strengths of the various models were determined using the ABAQUS
[1.27] finite element program. Three-dimensional brick elements
(C3D20 and C3D15) were employed with elastic�perfectly plastic
155Examples of Finite Element Models of Metal Tubular Connections
material properties being used in the finite element analysis. It was shown
that chord length and boundary conditions can have a significant influ-
ence on static collapse loads.
Saidani [7.10] investigated the effect of joint eccentricity on the local
and overall behavior of truss girders made from RHS members. Three
typical truss girders with identical general layout and comprising different
joint eccentricities were analyzed. Different numerical models of analysis
were presented and the implications for design were discussed. Only half
of each truss was analyzed due to the symmetry in loading and boundaryconditions. It was shown that the connection eccentricity can have signif-
icant effects on the axial force distribution in the bracings. However, its
influence on the overall truss deflection was negligible. Lee [7.11]
reviewed the numerical modeling techniques used in the finite element
analysis of tubular joints and provided guidance on obtaining information
on strength, stress fields, and stress intensity factors. Several commercial
software packages were compared in the mesh generation of complex
intersections of tubular member. For strength analysis, guidance was given
on model discretization, choice of elements, material properties input,
and weld modeling for valid results and modeling limitations. For stress
analysis, guidance was given on the extraction of stresses by using
different types of elements, weld modeling, and the use of submodeling
techniques for fatigue calculations. For fracture analysis, guidance was
given on the use of line-spring elements in shell models, the choice of
solid elements, cracked mesh generation, and interpretation of stress
intensity factors from finite element outputs.
Choo et al. [7.12] presented a new approach in the definition of joint
strength for thick-walled CHS X-joint subjected to brace axial loading. The
finite element models were created using MSC/PATRAN [7.4], and the
nonlinear analysis incorporating geometric and material nonlinearities was
carried out using the general-purpose finite element software ABAQUS
[1.27]. Nonlinear material property for the numerical study was based on
the true stress�strain curve represented by piecewise linear relations.
Twenty- quadratic solid elements with reduced integration (C3D20R) given
in the ABAQUS [1.27] were consistently used for modeling the brace,
chord, and weld regions. For thick-walled joints, four layers of elements
were employed across the chord and brace wall thickness, while for thin-
walled joints, two layers of elements were specified. For X-joint under brace
axial load, one-eighth of the entire joint was simulated with proper bound-
ary conditions applied on the symmetry planes. A new approach in the
156 Finite Element Analysis and Design of Metal Structures
definition of joint strength based on the plastic load approach with a consis-
tent coefficient λ was found to provide consistent correlation with the peak
loads in the joint load�deformation curve. The joint strength predicted
using the present approach was also compared with that obtained from the
current design recommendations for thick-walled CHS X-joint.
Karamanos and Anagnostou [7.13] presented nonlinear finite element
model to investigate the influence of external hydrostatic pressure on the
ultimate capacity of uniplanar X- and T-welded tubular connections
under axial and bending loads. The general-purpose finite element
program ABAQUS [1.27] was employed for the simulation and the
nonlinear analysis of tubular joint. A nonstructured mesh of finite ele-
ments was constructed, using a 20-node three-dimensional solid element
with reduced integration (C3D20R with 23 23 2 Gauss point grid).
Only one-eighth of the tubular X-joint was modeled with appropriate
symmetry conditions on the symmetry edges. The finite element meshes
are quite fine in the vicinity of the weld profile due to the strain concen-
trations and the occurrence of plastic deformations, but are rather coarse
away from the weld. Two elements were used through the tube thickness
to accurately simulate tube wall bending. Both geometric and material
nonlinearities were considered in the finite element analysis. Inelastic
effects on the response were taken into account through von Mises large
strain plasticity model with isotropic hardening. The nonlinear analysis
was conducted using a displacement-controlled marching scheme to trace
unstable equilibrium paths that exhibit “snap-back.” Good agreement
between the numerical results and test data was found. It was shown that
external pressure causes structural instability and has significant effects on
both the ultimate load and the deformation capacity of the joints. A simple
analytical formulation was developed to yield closed-form expressions for
the load�deformation relationship, which approximated the elastic�plastic
response of a pressurized tubular X-joint under axial loads.
Gho et al. [7.14] presented the experimental and numerical results of
the ultimate load behavior of CHS tubular joints with complete overlap
of braces. The finite element package MARC [7.2] with pre- and post-
processing program MENTAT was adopted for the simulation. The
mid-surface of the wall thickness of joint members was modeled using
doubly curved 4-node thick shell elements (MARC element type 75),
which can be used to consider the effect of transverse shear deformation.
Only one-half of the joint was modeled due to the symmetrical geometry
and boundary conditions. Fine meshes were used at the intersections of
157Examples of Finite Element Models of Metal Tubular Connections
members and the gap region of the joint to account for the effect of high
stress gradients. Both material and geometric nonlinearities were included
in the finite element analysis. The von Mises yield criterion and the mul-
tilinear isotropic work hardening rule of plasticity were applied. The large
displacement, the updated Lagrange procedure, and the finite strain plas-
ticity were activated in the analysis for complete large strain plasticity
formulation. A full Newton�Raphson method was adopted to reassemble
the stiffness matrix at each of the iteration. A modified Riks�Ramm
method was adopted in the loading application. A mesh convergence
study was performed to obtain optimum mesh size. A detailed para-
metric study including 1296 FE models was conducted by using the
verified finite element model to examine the failure modes and the
load�deformation characteristics of the joint. There were four possible
failure modes of the joint under lap brace axial compression. A combina-
tion of these failure modes can occur depending on the geometrical para-
meters of the joints.
Van Der Vegte et al. [7.15] conducted extensive numerical research
into the chord stress effect of CHS uniplanar K-, T-, and X-joints. The
study presented the results of finite element analyses on CHS uniplanar
X-joints under axial brace load with the chord subjected to either axial
load, in-plane bending moment or combinations of axial load and in-
plane bending moment. A new strength formulation was established for
X-joints under axial brace load solely. A chord stress function was
derived, describing the combined effect of axial chord load and in-plane
bending chord moment on the ultimate strength of uniplanar X-joints.
Gho and Yang [7.16] presented both experimental and numerical
investigations on CHS tubular joint with complete overlap of braces.
A doubly curved thick shell element (Type 75) given in the finite element
package MARC [7.2] was used to model the midface of members of the
joint, which took the transverse shear deformation effect into consider-
ation. The weld was also carefully modeled as a ring of shell elements
around the joint intersection. Only one-half of the joint was modeled in
view of the symmetrical properties of geometry and boundary conditions.
The fine meshes were created at the joint intersections and the short seg-
ment of through brace to account for the effect of high stress gradients.
The convergence study by varying the mesh density at joint intersections
was also conducted to obtain the optimum mesh size. The nonlinearity of
material and geometrical properties of the joint was included in the finite
element analysis. The von Mises yield criterion and the multilinear
158 Finite Element Analysis and Design of Metal Structures
isotropic work hardening rule of plasticity were applied. The large dis-
placement, the updated Lagrange procedure, and the finitestrain plasticity
were all activated for complete large strain plasticity formulation. A full
Newton�Raphson method was adopted to reassemble the stiffness matrix
at each of iteration. A modified Riks�Ramm method was employed in
the loading application. The finite element model was verified against the
current and previous test results with good agreement. A parametric
equation for the prediction of ultimate joint strength was developed based
on 3888 finite element models in the parametric study. It was found that
the ultimate joint strength was not significantly affected by the boundary
conditions and the chord prestresses. However, the ultimate joint strength
decreased with increasing gap size.
Shao et al. [7.17] studied the effect of the chord reinforcement on the
static strength of welded tubular T-joints by using the finite element
method. Twenty-Node hexahedral solid elements were used to model
brace and chord members as well as the butt weld connecting the tubes
with different thicknesses. The mesh around the weld toe was refined,
while a relatively coarse mesh was used far away from the weld toe to
increase the computational efficiency and obtain accurate numerical
results. Six layers of elements were employed in the thickness direction of
the chord reinforced region around the weld toe to consider the high
stress concentration in this region, while two layers of elements were used
in the regions far away from the weld toe to save computational time.
The residual stresses in the heat-affected region of the T-joint were not
considered in the finite element analysis. It was found that the static
strength can be greatly improved by increasing the chord thickness near
the intersection. However, it is ineffective to improve the static strength
by increasing the length of the reinforced chord. Furthermore, a paramet-
ric study of 240 T-joints was performed to investigate the effects of the
geometrical parameters and the chord thickness on the static strength of
the T-joints. A parametric equation was proposed to predict the static
strength of the tubular T-joint subjected to axial compression.
Van der Vegte et al. [7.18] reviewed the nonlinear finite element anal-
yses in the field of tubular structures. The main aspects of finite element
analyses for welded hollow section joints were overall discussed, which
include the solution technique such as implicit versus explicit methods,
choice of element type, material nonlinearity, modeling of the welds, and
limitations in predicting certain failure modes. The main difference
between the implicit and explicit solvers was further highlighted in terms
159Examples of Finite Element Models of Metal Tubular Connections
of the solution strategy and application as well as the effect of mesh
refinement on computational time and memory requirements, which was
also illustrated in the given examples. Liu and Deng [7.19] studied the
effect of out-of-plane bending performance of CHS X-joints by using
finite element analysis. Three-node triangular shell elements with reduced
integration (S3R) given in the ABAQUS [1.27] were used to model the
center region, while 4-node shell elements with reduced integration
(S4R) were used to model the other regions and the end plates of the
chord. The Riks method was used to consider effect of geometrically
nonlinear performance while the ideal elasto-plastic constitutive model
was employed. The finite element model was verified to be credible by
comparing with the experimental results. The influence of brace inclina-
tion angles, axial stress and diameter-to-thickness ratio of chord on failure
mode, ultimate bearing capacity, and flexural rigidity of tubular joints
were all investigated in the parametric study. It was found that a larger
brace inclination angle could increase the ultimate capacity of X-joint but
could decrease its flexural rigidity. Furthermore, axial compression and
tension in chords could weaken the rigidity and bearing capacity of
X-joints, and a considerable axial compression could lower the ductility
of X-joints.
7.3. EXPERIMENTAL INVESTIGATIONS OF METAL TUBULAR
CONNECTIONS
7.3.1 General
The experimental investigation, presented in this chapter and used for the
verification of the following finite element models, was conducted by
Feng and Young [7.20,7.21] on cold-formed stainless steel tubular T- and
X-joints. The test specimens were fabricated from SHS and RHS brace
and chord members. Both high strength stainless steel (duplex and high
strength austenitic) and normal strength stainless steel (AISI 304) speci-
mens were tested. Special attention was given to the deformations of
stainless steel tubular joints, which were generally larger than those of car-
bon steel tubular joints. The test strengths, flange indentation, and web
deflection of chord members, as well as the observed failure modes for all
test specimens were obtained. The tests were well designed and instru-
mented, which agrees with the criteria of a successful test programs set in
Section 1.3.
160 Finite Element Analysis and Design of Metal Structures
7.3.2 Scope
The design of the test program has accounted for most of the parameters
affecting the behavior of tubular joints. Looking at the strength of stainless
steel tubular joints, which depends mainly on (i) the ratio of brace width
to chord width (β5 b1/b0), (ii) the ratio of brace thickness to chord
thickness (τ5 t1/t0), (iii) the ratio of chord width to chord thickness
(2γ5 b0/t0), and (iv) the compressive preload (Np) applied to the chord
members. Therefore, the tests were conducted by applying axial compres-
sion force to the brace members using different values of β ranged from
0.5 to 1.0 (full width joint), τ from 0.5 to 2.0, and 2γ from 10 to 50,
which is beyond the validity range of most current design specifications
for tubular connections (2γ# 35). Three different levels of compressive
preload were applied to the chord members of the stainless steel tubular
X-joints. The effect of compressive chord preload on the strength of
stainless steel tubular X-joint was evaluated.
7.3.3 Test Specimens
The compression tests were performed on cold-formed stainless steel
tubular T- and X-joints of SHS and RHS. A total of 22 stainless steel
tubular T-joints and 32 stainless steel tubular X-joints was tested with
axial compression force applied to the brace members, in which 21 stain-
less steel tubular X-joints were tested with compressive preload applied to
the chord members. All test specimens were fabricated with brace mem-
bers fully welded at right angle to the center of the continuous chord
members.
The welded SHS and RHS consisted of a large range of section sizes.
For the chord members, the tubular hollow sections have nominal overall
flange width (b0) ranged from 40 to 200 mm, nominal overall depth of
the web (h0) from 40 to 200 mm, and nominal thickness (t0) from 1.5 to
6.0 mm. For the brace members, the tubular hollow sections have nomi-
nal overall flange width (b1) ranged from 40 to 150 mm, nominal overall
depth of the web (h1) from 40 to 200 mm, and nominal thickness (t1)
from 1.5 to 6.0 mm. The nominal wall thickness of both chord and brace
members go beyond the limits of the current design specifications, in
which the nominal wall thickness of hollow sections should not be less
than 2.5 mm. The length of the chord member (L0) was chosen as
h11 5h0 to ensure that the stresses at the brace and chord intersection are
not affected by the ends of the chord. This is because the points of
161Examples of Finite Element Models of Metal Tubular Connections
contra-flexure on the chord due to the applied load and reactions occur
sufficiently far away from the intersection region. The length of the brace
member (L1) was chosen as 2.5h1 to avoid the overall buckling of brace
members, which cannot reveal the true ultimate capacity of the tubular
joints. The measured crosssection dimensions of the test specimens are
summarized in Refs [7.20,7.21] using the nomenclature defined in
Figures 7.4�7.7.
Welds 
Seam weld
Seam weld
Weld 
Brace Brace
Chord
Chord
w'
t0
b0 h0 h0
b1
L0/2
L1
h1
w
w
h1/2
h1
t1 b1
r0
r0
w'
r1
(A) (B)
Figure 7.4 Definition of symbols for stainless steel tubular T-joint [7.20]. (A) End
view. (B) Elevation.
Brace 
Chord
Seam welds
Weld 
t0
h0
b0
L0
h1
t1
b1
L1
r1
r0
Figure 7.5 Three-dimensional view of stainless steel tubular T-joint [7.20].
162 Finite Element Analysis and Design of Metal Structures
7.3.4 Material Properties of Stainless Steel Tubes
As mentioned previously in Section 1.3, the successful test program
should carefully measure the material properties of all the test specimen
components. Hence, the presented test specimens in this chapter were
Welds 
Seam weld
Seam weld
w'
Welds 
Weld 
Brace Brace
Brace 
Chord
Brace 
Chord
(A) (B)
w'
t0
b0 h0
b1
r0
r0
L0/2
L1
h1
w
w
h1/2
h1
t1
w'
b1
h0
r1
Figure 7.6 Definition of symbols for stainless steel tubular X-joint [7.21]. (A) End
view. (B) Elevation.
Brace
Chord
Brace
Seam welds
Weld
t0
h0
b0
L0
h1
t1
b1
L1
r1
r0
Figure 7.7 Three-dimensional view of stainless steel tubular X-joint [7.21].
163Examples of Finite Element Models of Metal Tubular Connections
cold-rolled from austenitic stainless steel type AISI 304 (EN 1.4301), high
strength austenitic (HSA), and duplex (EN 1.4462) stainless steel sheets.
The stainless steel type AISI 304 is considered as normal strength mate-
rial, whereas the HSA and duplex are considered as high strength mate-
rial. The brace and chord members with the same dimensions were
selected from the same batch of tubes and so could be expected to have
similar material properties. In this study, the stainless steel tubes were
obtained from the same batch of specimens conducted by Zhou and
Young [7.22] for flexural members. The material properties of the stain-
less steel tubes were determined by tensile coupon tests, which include
the initial Young’s modulus (E), the proportional limit stress (σp), the
static 0.1% (σ0.1), 0.2% (σ0.2), 0.5% (σ0.5), and 1.0% (σ1.0) tensile proof
stresses, the static ultimate tensile stress (σu), and the elongation after frac-
ture (εf) based on a gauge length of 50 mm.
7.3.5 Test Rig and Procedure
7.3.5.1 Stainless Steel Tubular T-Joints
Once again, as mentioned previously in Section 1.3, the successful test
program should carefully look into the details of the test rig, positions,
and types of instrumentations as well as the test procedures in order to
capture all the significant and required test results. The schematic sketches
of the test arrangement presented in this book are shown in Figure 7.8A
and B, for the end view and elevation, respectively. Axial compression
force was applied to the test specimen by using a servo-controlled hydrau-
lic testing machine. The upper end support was movable to allow tests to
be conducted at various specimen dimensions. A special fixed-ended
bearing was used at the end of the brace member so that a uniform axial
compression load can be applied to the test specimen. The special bearing
was connected to the upper end support. The chord member of the test
specimen rests on the bottom end plate, which is connected to the bot-
tom support of the testing machine. This provided support to the entire
chord member.
Two displacement transducers were positioned on either side of the
brace member measuring the vertical deflections at the center of the con-
necting face of the chord. The transducers were positioned 20 mm away
from the faces of the brace member, as shown in Figure 7.9. The flange
indentation (u) in the chord member was obtained from the average read-
ing of these two transducers. For the stainless steel tubular T-joint tests, it
was observed that the maximum outward deflection (v) of the chord web
164 Finite Element Analysis and Design of Metal Structures
does not occur at the center of the chord sidewall. It may approximately
appear near the two-thirds of the overall depth of the chord web (h0).
The exact location of the maximum deformation of the chord sidewall
cannot be easily predicted, as it depends on the initial plate imperfection
of the chord sidewall. Hence, two displacement transducers were posi-
tioned at the center of the chord sidewall to record the deflection. The
average of these readings was also taken as the chord web deflection (v),
as shown in Figure 7.9. Two other displacement transducers were posi-
tioned diagonally on the bottom end plate to measure the axial shortening
of the test specimen.
Bottom support
Bottom end plate
Specimen
Loading ram
Movable upper end support
Transducer (u)
Vertical bolt
Top end plate
Special fixed-ended bearing
Transducer (v)
(A)
Transducer (v)
Bottom support
Bottom end plate
Vertical bolt
Specimen
Transducer (u)
Loading ram
Movable upper end support
Special fixed-ended bearing
Top end plate
(B)
Figure 7.8 Schematic sketch of stainless steel tubular T-joint tests [7.20]. (A) End
view. (B) Elevation.
165Examples of Finite Element Models of Metal Tubular Connections
A 1000-kN capacity servo-controlled hydraulic testing machine was
used to apply axial compression force to the test specimen. Displacement
control was used to drive the hydraulic actuator at a constant speed of
0.2 mm/min for full width tubular T-joints and 0.4 mm/min for other
tubular T-joints. The use of displacement control allowed the tests to be
continued in the post-ultimate range. The applied loads and readings of
displacement transducers were recorded automatically at regular interval
by using a data acquisition system. A photograph of a typical test setup of
stainless steel tubular T-joint of specimen TD-C1603 3-B1603 3 is
shown in Figure 7.10.
7.3.5.2 Stainless Steel Tubular X-Joints Without Chord Preload
Figure 7.11A and B shows the schematic sketches of the test arrangement
of stainless steel tubular X-joints without chord preload for the end view
and elevation, respectively. The test rig and procedure were employed
similarly as previously detailed for the T-joints. The top end plate was
bolted to the upper end support, which was considered to be a fixed-
ended boundary condition. The load was applied to the bottom brace of
the test specimen through a special fixed-ended bearing.
Four displacement transducers were positioned on either side of the
brace members measuring the vertical deflections at the center of the con-
necting faces of the chord. The transducers were positioned 20 mm away
from the faces of the brace members, as shown in Figure 7.12. The flange
indentation (u) for one face of the chord member was obtained from these
transducers. Two displacement transducers were positioned at the center of
the chord sidewall to record the deflection. The average of these readings
was also taken as the chord web deflection (v), as shown in Figure 7.12.
Transducers (u)
u
v
Transducer (u)
Transducers (v)
20 mm 20 mm
Transducer (v)
(A) (B)
Figure 7.9 Deformations of stainless steel tubular T-joint [7.20]. (A) End view. (B)
Elevation.
166 Finite Element Analysis and Design of Metal Structures
Two other displacement transducers were positioned diagonally on the
bottom end plate to measure the axial shortening of the test specimen.
Axial compression force was applied to the braces of the stainless steel
tubular X-joints using the same servo-controlled hydraulic testing
machine as that used for the tests of stainless steel tubular T-joints.
Displacement control was used to drive the hydraulic actuator at a
constant speed of 0.2 mm/min for full width tubular X-joints, and
0.4 mm/min for other tubular X-joints. The applied loads and readings
of displacement transducers were recorded automatically at regular inter-
val by using the same data acquisition system. A photograph of a typicaltest setup of stainless steel tubular X-joint without chord preload of speci-
men XH-C2003 4-B2003 4-P0 is shown in Figure 7.13.
7.3.5.3 Stainless Steel Tubular X-Joints with Chord Preload
Similar test rig and nearly the same instrumentation were used for the
tests of stainless steel tubular X-joints with chord preload. However, four
high strength steel bars were used to apply the compressive preload to the
Figure 7.10 Test setup of stainless steel tubular T-joint of specimen TD-
C1603 3-B1603 3.
167Examples of Finite Element Models of Metal Tubular Connections
chord members. The ENERPAC of 1000 kN capacity hydraulic jack was
used at one end of the chord members to apply a specified compressive
preload (Np). A load cell was positioned at the other end of the chord
member to monitor the applied compressive preload. The schematic
sketches of the test arrangement of stainless steel tubular X-joints with
chord preload are shown in Figure 7.14A and B for the end view and ele-
vation, respectively. Four single-element strain gauges with a gauge length
of 5 mm (TML FLA-5-17) specific for stainless steel were attached at the
middle length between the chord end and the face of the brace members
Transducer (v)
Bottom support
Bottom end plate
Top end plate
Special fixed-ended bearing
Vertical bolt
Specimen
Loading ram
Movable upper end support
Transducers (u)
(A)
Transducer (v)
Bottom support
Special fixed-ended bearing
Bottom end plate
Vertical bolt
Horizontal bolt
Top end plate
Specimen
Transducer (u)
Loading ram
Movable upper end support
(B)
Figure 7.11 Schematic sketch of stainless steel tubular X-joint tests without chord
preload [7.21]. (A) End view. (B) Elevation.
168 Finite Element Analysis and Design of Metal Structures
in order to ensure the preload was uniformly applied to the chord mem-
ber. The strain gauges were located at the corners of the hollow sections,
as shown in Figure 7.14B. The hydraulic jack was continuously adjusted
to keep the preload at its initial value62% throughout the test.
Transducer (v)
Transducers (u)
u
v
Transducer (u)
Transducers (v)
20 mm 20 mm
(A) (B)
Figure 7.12 Deformations of stainless steel tubular X-joint [7.21]. (A) End view.
(B) Elevation.
Figure 7.13 Test setup of stainless steel tubular X-joint without chord preload of
specimen XH-C2003 4-B2003 4-P0.
169Examples of Finite Element Models of Metal Tubular Connections
The nominal preloads used in the tests were 10%, 30%, and 50% of the
yield load (A0σ0.2) of the chord members. Axial compression force was
applied to the braces of the test specimen using the same servo-controlled
hydraulic testing machine. The same fixed-ended bearing as that used for
the tests of stainless steel tubular T-joints was positioned at the upper end
to ensure a uniform axial compression force applied to the braces.
Displacement control was used to drive the hydraulic actuator at a con-
stant speed of 0.1 mm/min for full width tubular X-joints, and 0.2 mm/min
Bottom support
Bottom end plate
Specimen
Loading ram
Movable upper end support
Transducers (u) Transducer (v)
Special fixed-ended bearing
Vertical bolt
Top end plate
(A)
Transducer (v)
Bottom support
Bottom end plate
Specimen
Loading ram
Steel plates
Bolts
Load cell
High strength steel bars
Hydraulic jack A
A
A-A
Strain gauges
Transducer (u)
Vertical bolt
Movable upper end support
Special fixed-ended bearing
Top end plate
(B)
Figure 7.14 Schematic sketch of stainless steel tubular X-joint tests with chord pre-
load [7.21]. (A) End view. (B) Elevation.
170 Finite Element Analysis and Design of Metal Structures
for other tubular X-joints. The same measurement system as that used for
the tests of stainless steel tubular X-joints without chord preload was
employed to obtain the chord flange indentation (u), the chord web deflec-
tion (v), and the axial shortening of the test specimens. The same data acqui-
sition system was also used during the tests to record the applied loads and
readings of displacement transducers manually when the compressive pre-
loads were within the range of the specified values. A photograph of a typical
test setup of stainless steel tubular X-joint with chord preload of specimen
XH-C2003 4-B2003 4-P0.1 is shown in Figure 7.15.
7.4. FINITE ELEMENT MODELING OF METAL TUBULAR
CONNECTIONS
7.4.1 General
The test results given in Refs [7.20,7.21] have provided enough informa-
tion for the verification of finite element models developed by Feng and
Young [7.23]. The developed models for cold-formed stainless steel tubular
Figure 7.15 Test setup of stainless steel tubular X-joint with chord preload of speci-
men XH-C2003 4-B2003 4-P0.1.
171Examples of Finite Element Models of Metal Tubular Connections
T- and X-joints of SHS and RHS used the general-purpose finite element
program ABAQUS [1.27]. Three finite element models were developed,
namely, the T-joints, X-joints, and X-joints with chord preload, including
various critical influential factors, such as modeling of materials and welds,
contact interaction between the T-joint specimens and the supporting
plate, as well as loading and boundary conditions. The load�displacement
nonlinear analysis was performed by using the (�STATIC) procedure avail-
able in the ABAQUS [1.27] library. Both geometric and material nonlinea-
rities have been taken into account in the finite element models. The
element type and mesh size of the stainless steel tube and the welding
material were carefully determined by the convergence studies to provide
accurate results with reasonable computational cost. The joint strengths,
failure modes, and load�deformation curves of stainless steel tubular joints
were all obtained from the finite element analysis.
A 4-node doubly curved shell element with reduced integration
(S4R) has been used by many researchers to model the brace and chord
members of welded tubular joints. A 5-point integration was applied
through the shell thickness with full complement of six degrees of free-
dom per node. The S4R element provides accurate solution to most
applications by allowing for transverse shear deformation, which is impor-
tant for the simulation of thick shell element. However, the shell element
in the contact algorithm could incorrectly allow penetration of one mem-
ber into the other due to its ignorance of physical thickness of the ele-
ment. Therefore, three-dimensional 8-node solid element with reduced
integration (C3D8R) was used in this study to model the cold-formed
stainless steel tubular joints. This element is fully isoparametric with first-
order interpolation. The use of solid element rather than shell element
for the modeling of welded tubular joints could achieve accurate results
with slight increase of computational time.
In order to obtain the optimum finite element mesh size, the conver-
gence studies were carried out. It was found that the mesh size of approx-
imately 33 3 mm (length by width) for small specimens, 63 6 mm for
medium specimens, and 103 10 mm for large specimens in modeling the
flat portions of both flange and web elements could achieve accurate
results with the minimum computational time. The corresponding
length-to-width ratio of the elements is equal to 1.0 for both brace and
chord members. A finer mesh of four elements was used at the corner
portions due to their importance in transferring the stress from the flange
to the web. Based on the study of Choo et al. [7.12], four layers of solid
elements were employed across the tube wall thickness for thick-walled
172 Finite Element Analysis and Design of Metal Structures
tubular members (b0/t0# 20 for chord member; and b1/t1# 20 for brace
member), while two layers of solid elements were used for thin-walled
tubular members (b0/t0. 20 for chord member; and b1/t1. 20 for brace
member). This technique was implemented through the thickness of all
tubular members to provide